XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Reinforced Concrete Beam in Ansys Workbench
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Fri Jul 11, 2014 1:28 am  Reply with quote

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would like my beam be 3d element(solid65) and the reinforcements LINK180 element. Is it possible that I could model? Can I see the crack pattern in the beam at the time of failure in ansys workbench?I would want to gradually increase the pressure and find the pressure at which it fails.When I do so, I get a convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-Universität Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Fri Jul 11, 2014 5:03 am  Reply with quote

Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rajendra.kachhadia
User


Joined: 02 Jul 2014
Posts: 9

PostPosted: Fri Jul 11, 2014 7:25 am  Reply with quote

Hello Rukmani,
You can use APDL to model it with link elements. However, I am not sure
these elements can be applied with failure criteria.

Rajendra
Desserve Engineering Solutions
www.desservees.com
info@desservees.com
fea@desservees.com
cfd@desservees.com
+919586307908

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Peter Barrett
Sent: Friday, July 11, 2014 5:33 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential
information of Computer Aided Engineering Associates. This e-mail is
intended solely for the use of the individual or entity to which it is
addressed. If you are not the intended recipient of this e-mail, you are
hereby notified that any copying, distribution, dissemination or action
taken in relation to the contents of this e-mail and any of its attachments
is strictly prohibited and may be unlawful. If you have received this e-mail
in error, please notify the sender immediately and permanently delete the
original e-mail and destroy any copies or printouts of this e-mail as well
as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Fri Jul 11, 2014 7:45 am  Reply with quote

Rukmani,

You can't create failure directly in the links unless you use some kind of
"ekill" option based on a strain value for example. However, I don't think
that is necessary. I would recommend defining a nonlinear stress-strain
curve such that when the rebar yields it will lose most of its strength and
this should be adequate in your case. The other "failure" issue to deal with
would be debonding between the concrete and steel. This could be modeled
with ANSYS beam-to-beam contact, but again probably not something that is
significant relative to all the other assumptions needed and usually is
neglected with this type of modeling.

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of FEA
Sent: Friday, July 11, 2014 10:25 AM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hello Rukmani,
You can use APDL to model it with link elements. However, I am not sure
these elements can be applied with failure criteria.

Rajendra
Desserve Engineering Solutions
www.desservees.com
info@desservees.com
fea@desservees.com
cfd@desservees.com
+919586307908

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Peter Barrett
Sent: Friday, July 11, 2014 5:33 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential
information of Computer Aided Engineering Associates. This e-mail is
intended solely for the use of the individual or entity to which it is
addressed. If you are not the intended recipient of this e-mail, you are
hereby notified that any copying, distribution, dissemination or action
taken in relation to the contents of this e-mail and any of its attachments
is strictly prohibited and may be unlawful. If you have received this e-mail
in error, please notify the sender immediately and permanently delete the
original e-mail and destroy any copies or printouts of this e-mail as well
as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Sat Jul 12, 2014 8:22 am  Reply with quote

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65
element and reinforcements with link180 elements and asssigned these
following properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using
these commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But
as I need to see the crack patterns , I transfered the DS.DAT from WB
to ansys mechanical APDL. I can see the element solutions, But unable
to see the cracks at each step.Could you please tell me How I could
solve this problem and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Mon Jul 14, 2014 6:07 am  Reply with quote

Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not write all
the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65 element
and reinforcements with link180 elements and asssigned these following
properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using these
commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But as I
need to see the crack patterns , I transfered the DS.DAT from WB to ansys
mechanical APDL. I can see the element solutions, But unable to see the
cracks at each step.Could you please tell me How I could solve this problem
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Tue Jul 15, 2014 3:36 am  Reply with quote

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in
my beam. I can even send my dat.ds file. I really cant find where the
problem is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not write all
the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65 element
and reinforcements with link180 elements and asssigned these following
properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using these
commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But as I
need to see the crack patterns , I transfered the DS.DAT from WB to ansys
mechanical APDL. I can see the element solutions, But unable to see the
cracks at each step.Could you please tell me How I could solve this problem
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Tue Jul 15, 2014 6:33 am  Reply with quote

Rukmani,

Seems to work fine for me in REV 15 using the following input file:

/PREP7
/TITLE, VM146, BENDING OF A REINFORCED CONCRETE BEAM
C*** STR. OF MATL., TIMOSHENKO, PART 1, 3RD ED., PAGE 221

ANTYPE,STATIC
ET,1,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
ET,2,LINK180 ! STEEL RODS
ET,3,PIPE288 ! DUMMY ELEMENTS FOR CONSTRAINT EQUATIONS
KEYOPT,3,3,3 ! CUBIC SHAPE FUNCTION
KEYOPT,3,4,2 ! THICK PIPE THEORY
R,1
SECTYPE,2,LINK
SECDATA,0.15 ! HALF AREA OF ROD
SECTYPE,3,PIPE
SECDATA,1,0.5,8
MP,EX,1,2E6 ! CONCRETE PROPERTIES
MP,NUXY,1,0
TB,CONCR,1
TBDATA,3,0.0,-1 ! ZERO TENSILE CRACKING STRENGTH
! REMOVE CRUSHING CAPABILITY
MP,EX,2,30E6 ! STEEL PROPERTIES
MP,NUXY,2,0.3
N,1
N,2,1.5
NGEN,5,2,1,2,1,,1.5
NGEN,2,10,1,10,1,,,5
E,7,8,10,9,17,18,20,19
TYPE,3 ! DEFINE DUMMY ELEMENTS FOR ROTZ DOF
SECNUM,3
E,10,8
E,20,18
EGEN,4,-2,1,3

TYPE,2
MAT,2 ! REINFORCING RODS AT THE BOTTOM SURFACE
SECNUM,2
E,1,2
E,11,12
CE,1,, 2,UX,-1, 6,UX,1, 6,ROTZ,3 ! CONSTRAINT EQUATION TO ENSURE
CE,2,,12,UX,-1,16,UX,1,16,ROTZ,3 ! PLANE SECTION REMAINS PLANE
CE,3,, 4,UX,-1, 6,UX,1, 6,ROTZ,1.5
CE,4,,14,UX,-1,16,UX,1,16,ROTZ,1.5
CE,5,, 8,UX,-1, 6,UX,1, 6,ROTZ,-1.5
CE,6,,18,UX,-1,16,UX,1,16,ROTZ,-1.5
CE,7,,10,UX,-1, 6,UX,1, 6,ROTZ,-3
CE,8,,20,UX,-1,16,UX,1,16,ROTZ,-3
NSEL,S,LOC,X
D,ALL,ALL ! FIX NODES IN Y-Z PLANE
NSEL,ALL
D,ALL,ROTY ! CONSTRAIN UNNEEDED PIPE ROTATIONS
F,6,MZ,300,,16,10 ! APPLY BENDING MOMENT
FINISH
/SOLU
AUTOTS,ON
NSUBST,5
OUTPR,,LAST
/OUT,SCRATCH
SOLVE
/POST1
!
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/REPLO
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack





Peter Barrett, P.E.
Vice President
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Tuesday, July 15, 2014 5:26 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in my
beam. I can even send my dat.ds file. I really cant find where the problem
is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not write
all the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Quote:
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65 element
and reinforcements with link180 elements and asssigned these following
properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using these
commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But as I
need to see the crack patterns , I transfered the DS.DAT from WB to ansys
mechanical APDL. I can see the element solutions, But unable to see the
cracks at each step.Could you please tell me How I could solve this
problem
Quote:
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get
a
Quote:
Quote:
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Tue Jul 15, 2014 8:17 am  Reply with quote

Peter Barrett,

Thank you very much.
But for this case it works for me too.But when I model it in ansys
workbench and then take the dat.ds file to ansys mechancial apdl, I
cant see the cracks.
If I model the same model in ansys apdl , then I could see the
cracks. But I want to advance my model in the future. So I want to
work in ansys workbench,and still see the cracks.

Do you think , I could do it?

Thanks adn Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Seems to work fine for me in REV 15 using the following input file:

/PREP7
/TITLE, VM146, BENDING OF A REINFORCED CONCRETE BEAM
C*** STR. OF MATL., TIMOSHENKO, PART 1, 3RD ED., PAGE 221

ANTYPE,STATIC
ET,1,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
ET,2,LINK180 ! STEEL RODS
ET,3,PIPE288 ! DUMMY ELEMENTS FOR CONSTRAINT EQUATIONS
KEYOPT,3,3,3 ! CUBIC SHAPE FUNCTION
KEYOPT,3,4,2 ! THICK PIPE THEORY
R,1
SECTYPE,2,LINK
SECDATA,0.15 ! HALF AREA OF ROD
SECTYPE,3,PIPE
SECDATA,1,0.5,8
MP,EX,1,2E6 ! CONCRETE PROPERTIES
MP,NUXY,1,0
TB,CONCR,1
TBDATA,3,0.0,-1 ! ZERO TENSILE CRACKING STRENGTH
! REMOVE CRUSHING CAPABILITY
MP,EX,2,30E6 ! STEEL PROPERTIES
MP,NUXY,2,0.3
N,1
N,2,1.5
NGEN,5,2,1,2,1,,1.5
NGEN,2,10,1,10,1,,,5
E,7,8,10,9,17,18,20,19
TYPE,3 ! DEFINE DUMMY ELEMENTS FOR ROTZ DOF
SECNUM,3
E,10,8
E,20,18
EGEN,4,-2,1,3

TYPE,2
MAT,2 ! REINFORCING RODS AT THE BOTTOM SURFACE
SECNUM,2
E,1,2
E,11,12
CE,1,, 2,UX,-1, 6,UX,1, 6,ROTZ,3 ! CONSTRAINT EQUATION TO ENSURE
CE,2,,12,UX,-1,16,UX,1,16,ROTZ,3 ! PLANE SECTION REMAINS PLANE
CE,3,, 4,UX,-1, 6,UX,1, 6,ROTZ,1.5
CE,4,,14,UX,-1,16,UX,1,16,ROTZ,1.5
CE,5,, 8,UX,-1, 6,UX,1, 6,ROTZ,-1.5
CE,6,,18,UX,-1,16,UX,1,16,ROTZ,-1.5
CE,7,,10,UX,-1, 6,UX,1, 6,ROTZ,-3
CE,8,,20,UX,-1,16,UX,1,16,ROTZ,-3
NSEL,S,LOC,X
D,ALL,ALL ! FIX NODES IN Y-Z PLANE
NSEL,ALL
D,ALL,ROTY ! CONSTRAIN UNNEEDED PIPE ROTATIONS
F,6,MZ,300,,16,10 ! APPLY BENDING MOMENT
FINISH
/SOLU
AUTOTS,ON
NSUBST,5
OUTPR,,LAST
/OUT,SCRATCH
SOLVE
/POST1
!
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/REPLO
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack





Peter Barrett, P.E.
Vice President
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Tuesday, July 15, 2014 5:26 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in my
beam. I can even send my dat.ds file. I really cant find where the problem
is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not write
all the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Quote:
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65 element
and reinforcements with link180 elements and asssigned these following
properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using these
commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But as I
need to see the crack patterns , I transfered the DS.DAT from WB to ansys
mechanical APDL. I can see the element solutions, But unable to see the
cracks at each step.Could you please tell me How I could solve this
problem
Quote:
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get
a
Quote:
Quote:
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Wed Jul 16, 2014 4:34 am  Reply with quote

Rukmani,

I was able to create crack plots in WB using the following three command
blocks:

1) In the Geometry solid branch:

ET,matid,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
MP,EX,matid,2E6 ! CONCRETE PROPERTIES
MP,NUXY,matid,0
TB,CONCR,matid
TBDATA,3,0.0,-1

2) In the Static Structural branch:

outres,all,all

3) In the Solution branch:

set,last
/show,png
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack



Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Tuesday, July 15, 2014 11:17 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thank you very much.
But for this case it works for me too.But when I model it in ansys workbench
and then take the dat.ds file to ansys mechancial apdl, I cant see the
cracks.
If I model the same model in ansys apdl , then I could see the cracks. But
I want to advance my model in the future. So I want to work in ansys
workbench,and still see the cracks.

Do you think , I could do it?

Thanks adn Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Seems to work fine for me in REV 15 using the following input file:

/PREP7
/TITLE, VM146, BENDING OF A REINFORCED CONCRETE BEAM
C*** STR. OF MATL., TIMOSHENKO, PART 1, 3RD ED., PAGE 221

ANTYPE,STATIC
ET,1,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
ET,2,LINK180 ! STEEL RODS
ET,3,PIPE288 ! DUMMY ELEMENTS FOR CONSTRAINT EQUATIONS
KEYOPT,3,3,3 ! CUBIC SHAPE FUNCTION
KEYOPT,3,4,2 ! THICK PIPE THEORY
R,1
SECTYPE,2,LINK
SECDATA,0.15 ! HALF AREA OF ROD
SECTYPE,3,PIPE
SECDATA,1,0.5,8
MP,EX,1,2E6 ! CONCRETE PROPERTIES
MP,NUXY,1,0
TB,CONCR,1
TBDATA,3,0.0,-1 ! ZERO TENSILE CRACKING STRENGTH
! REMOVE CRUSHING CAPABILITY
MP,EX,2,30E6 ! STEEL PROPERTIES
MP,NUXY,2,0.3
N,1
N,2,1.5
NGEN,5,2,1,2,1,,1.5
NGEN,2,10,1,10,1,,,5
E,7,8,10,9,17,18,20,19
TYPE,3 ! DEFINE DUMMY ELEMENTS FOR ROTZ DOF
SECNUM,3
E,10,8
E,20,18
EGEN,4,-2,1,3

TYPE,2
MAT,2 ! REINFORCING RODS AT THE BOTTOM SURFACE
SECNUM,2
E,1,2
E,11,12
CE,1,, 2,UX,-1, 6,UX,1, 6,ROTZ,3 ! CONSTRAINT EQUATION TO ENSURE
CE,2,,12,UX,-1,16,UX,1,16,ROTZ,3 ! PLANE SECTION REMAINS PLANE
CE,3,, 4,UX,-1, 6,UX,1, 6,ROTZ,1.5
CE,4,,14,UX,-1,16,UX,1,16,ROTZ,1.5
CE,5,, 8,UX,-1, 6,UX,1, 6,ROTZ,-1.5
CE,6,,18,UX,-1,16,UX,1,16,ROTZ,-1.5
CE,7,,10,UX,-1, 6,UX,1, 6,ROTZ,-3
CE,8,,20,UX,-1,16,UX,1,16,ROTZ,-3
NSEL,S,LOC,X
D,ALL,ALL ! FIX NODES IN Y-Z PLANE
NSEL,ALL
D,ALL,ROTY ! CONSTRAIN UNNEEDED PIPE
ROTATIONS
Quote:
F,6,MZ,300,,16,10 ! APPLY BENDING MOMENT
FINISH
/SOLU
AUTOTS,ON
NSUBST,5
OUTPR,,LAST
/OUT,SCRATCH
SOLVE
/POST1
!
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/REPLO
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack





Peter Barrett, P.E.
Vice President
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Sent: Tuesday, July 15, 2014 5:26 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in
my beam. I can even send my dat.ds file. I really cant find where the
problem is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not
write all the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Quote:
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65
element and reinforcements with link180 elements and asssigned these
following properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using
these commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But
as I need to see the crack patterns , I transfered the DS.DAT from WB
to ansys mechanical APDL. I can see the element solutions, But unable
to see the cracks at each step.Could you please tell me How I could
solve this
problem
Quote:
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get
a
Quote:
Quote:
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Wed Jul 16, 2014 6:56 am  Reply with quote

Mr.Peter Barrett,

Thank you very much for your help. I am able to view the cracks
now.Previously I had given the command "outres,all,all" under solutions.

Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

I was able to create crack plots in WB using the following three command
blocks:

1) In the Geometry solid branch:

ET,matid,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
MP,EX,matid,2E6 ! CONCRETE PROPERTIES
MP,NUXY,matid,0
TB,CONCR,matid
TBDATA,3,0.0,-1

2) In the Static Structural branch:

outres,all,all

3) In the Solution branch:

set,last
/show,png
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack



Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Tuesday, July 15, 2014 11:17 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thank you very much.
But for this case it works for me too.But when I model it in ansys workbench
and then take the dat.ds file to ansys mechancial apdl, I cant see the
cracks.
If I model the same model in ansys apdl , then I could see the cracks. But
I want to advance my model in the future. So I want to work in ansys
workbench,and still see the cracks.

Do you think , I could do it?

Thanks adn Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Seems to work fine for me in REV 15 using the following input file:

/PREP7
/TITLE, VM146, BENDING OF A REINFORCED CONCRETE BEAM
C*** STR. OF MATL., TIMOSHENKO, PART 1, 3RD ED., PAGE 221

ANTYPE,STATIC
ET,1,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
ET,2,LINK180 ! STEEL RODS
ET,3,PIPE288 ! DUMMY ELEMENTS FOR CONSTRAINT EQUATIONS
KEYOPT,3,3,3 ! CUBIC SHAPE FUNCTION
KEYOPT,3,4,2 ! THICK PIPE THEORY
R,1
SECTYPE,2,LINK
SECDATA,0.15 ! HALF AREA OF ROD
SECTYPE,3,PIPE
SECDATA,1,0.5,8
MP,EX,1,2E6 ! CONCRETE PROPERTIES
MP,NUXY,1,0
TB,CONCR,1
TBDATA,3,0.0,-1 ! ZERO TENSILE CRACKING STRENGTH
! REMOVE CRUSHING CAPABILITY
MP,EX,2,30E6 ! STEEL PROPERTIES
MP,NUXY,2,0.3
N,1
N,2,1.5
NGEN,5,2,1,2,1,,1.5
NGEN,2,10,1,10,1,,,5
E,7,8,10,9,17,18,20,19
TYPE,3 ! DEFINE DUMMY ELEMENTS FOR ROTZ DOF
SECNUM,3
E,10,8
E,20,18
EGEN,4,-2,1,3

TYPE,2
MAT,2 ! REINFORCING RODS AT THE BOTTOM SURFACE
SECNUM,2
E,1,2
E,11,12
CE,1,, 2,UX,-1, 6,UX,1, 6,ROTZ,3 ! CONSTRAINT EQUATION TO ENSURE
CE,2,,12,UX,-1,16,UX,1,16,ROTZ,3 ! PLANE SECTION REMAINS PLANE
CE,3,, 4,UX,-1, 6,UX,1, 6,ROTZ,1.5
CE,4,,14,UX,-1,16,UX,1,16,ROTZ,1.5
CE,5,, 8,UX,-1, 6,UX,1, 6,ROTZ,-1.5
CE,6,,18,UX,-1,16,UX,1,16,ROTZ,-1.5
CE,7,,10,UX,-1, 6,UX,1, 6,ROTZ,-3
CE,8,,20,UX,-1,16,UX,1,16,ROTZ,-3
NSEL,S,LOC,X
D,ALL,ALL ! FIX NODES IN Y-Z PLANE
NSEL,ALL
D,ALL,ROTY ! CONSTRAIN UNNEEDED PIPE
ROTATIONS
Quote:
F,6,MZ,300,,16,10 ! APPLY BENDING MOMENT
FINISH
/SOLU
AUTOTS,ON
NSUBST,5
OUTPR,,LAST
/OUT,SCRATCH
SOLVE
/POST1
!
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/REPLO
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack





Peter Barrett, P.E.
Vice President
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Sent: Tuesday, July 15, 2014 5:26 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in
my beam. I can even send my dat.ds file. I really cant find where the
problem is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not
write all the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Quote:
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65
element and reinforcements with link180 elements and asssigned these
following properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using
these commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But
as I need to see the crack patterns , I transfered the DS.DAT from WB
to ansys mechanical APDL. I can see the element solutions, But unable
to see the cracks at each step.Could you please tell me How I could
solve this
problem
Quote:
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get
a
Quote:
Quote:
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Wed Jul 16, 2014 7:09 am  Reply with quote

Hallo,

In ansys workbench, Is it possible to give the uni axial stress strain
data for the concrete iwth solid65 element instead of MISO stress and
strain properties and still see the cracks and crushing of concrete
under load?

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

I was able to create crack plots in WB using the following three command
blocks:

1) In the Geometry solid branch:

ET,matid,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
MP,EX,matid,2E6 ! CONCRETE PROPERTIES
MP,NUXY,matid,0
TB,CONCR,matid
TBDATA,3,0.0,-1

2) In the Static Structural branch:

outres,all,all

3) In the Solution branch:

set,last
/show,png
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack



Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Tuesday, July 15, 2014 11:17 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thank you very much.
But for this case it works for me too.But when I model it in ansys workbench
and then take the dat.ds file to ansys mechancial apdl, I cant see the
cracks.
If I model the same model in ansys apdl , then I could see the cracks. But
I want to advance my model in the future. So I want to work in ansys
workbench,and still see the cracks.

Do you think , I could do it?

Thanks adn Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Seems to work fine for me in REV 15 using the following input file:

/PREP7
/TITLE, VM146, BENDING OF A REINFORCED CONCRETE BEAM
C*** STR. OF MATL., TIMOSHENKO, PART 1, 3RD ED., PAGE 221

ANTYPE,STATIC
ET,1,SOLID65,,,,,2 ! REINFORCED CONCRETE SOLID ELEMENT
ET,2,LINK180 ! STEEL RODS
ET,3,PIPE288 ! DUMMY ELEMENTS FOR CONSTRAINT EQUATIONS
KEYOPT,3,3,3 ! CUBIC SHAPE FUNCTION
KEYOPT,3,4,2 ! THICK PIPE THEORY
R,1
SECTYPE,2,LINK
SECDATA,0.15 ! HALF AREA OF ROD
SECTYPE,3,PIPE
SECDATA,1,0.5,8
MP,EX,1,2E6 ! CONCRETE PROPERTIES
MP,NUXY,1,0
TB,CONCR,1
TBDATA,3,0.0,-1 ! ZERO TENSILE CRACKING STRENGTH
! REMOVE CRUSHING CAPABILITY
MP,EX,2,30E6 ! STEEL PROPERTIES
MP,NUXY,2,0.3
N,1
N,2,1.5
NGEN,5,2,1,2,1,,1.5
NGEN,2,10,1,10,1,,,5
E,7,8,10,9,17,18,20,19
TYPE,3 ! DEFINE DUMMY ELEMENTS FOR ROTZ DOF
SECNUM,3
E,10,8
E,20,18
EGEN,4,-2,1,3

TYPE,2
MAT,2 ! REINFORCING RODS AT THE BOTTOM SURFACE
SECNUM,2
E,1,2
E,11,12
CE,1,, 2,UX,-1, 6,UX,1, 6,ROTZ,3 ! CONSTRAINT EQUATION TO ENSURE
CE,2,,12,UX,-1,16,UX,1,16,ROTZ,3 ! PLANE SECTION REMAINS PLANE
CE,3,, 4,UX,-1, 6,UX,1, 6,ROTZ,1.5
CE,4,,14,UX,-1,16,UX,1,16,ROTZ,1.5
CE,5,, 8,UX,-1, 6,UX,1, 6,ROTZ,-1.5
CE,6,,18,UX,-1,16,UX,1,16,ROTZ,-1.5
CE,7,,10,UX,-1, 6,UX,1, 6,ROTZ,-3
CE,8,,20,UX,-1,16,UX,1,16,ROTZ,-3
NSEL,S,LOC,X
D,ALL,ALL ! FIX NODES IN Y-Z PLANE
NSEL,ALL
D,ALL,ROTY ! CONSTRAIN UNNEEDED PIPE
ROTATIONS
Quote:
F,6,MZ,300,,16,10 ! APPLY BENDING MOMENT
FINISH
/SOLU
AUTOTS,ON
NSUBST,5
OUTPR,,LAST
/OUT,SCRATCH
SOLVE
/POST1
!
!
/VIEW, 1, 0.684679427197 , 0.241361389380 , 0.687719973310
/ANG, 1, 0.136702653737
/REPLO
/SHOW,WIN32
/DEVICE,VECTOR,1
/DEVICE,BBOX,1
/DEVICE,DITHER,1
/DEVICE,ANIM,BMP
!
Plcrack





Peter Barrett, P.E.
Vice President
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Sent: Tuesday, July 15, 2014 5:26 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

Thanks for your reply. I even tried with this command "outres,all,all"
and " /DEVICE,VECTOR,1"

But still it doesnt work. I want to check out the crack probagation in
my beam. I can even send my dat.ds file. I really cant find where the
problem is.

It would be helpful if you could tell me.
I have attached my dat.ds file along with this mail.

--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Two things to try if PLCRACK is not working:

1) Make sure that you are writing all the results -- WB will not
write all the data by default. Add a command:

outres,all,all ! solution command

2) You might also want to switch to vector plotting to see inside the
elements:

/DEVICE,VECTOR,1


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani
Ganesan
Quote:
Sent: Saturday, July 12, 2014 11:22 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Respected All,

Thank you very much for your replies.

As Mr.Peter Barrett said I modelled my concrete beam with solid65
element and reinforcements with link180 elements and asssigned these
following properties in ansys workbench.

"
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0

MP,EX,MATID,24267.688
MP,NUXY,MATID,0.2


TB,MISO,MATID,1
TBTEMP,22
TBPT,DEFI,0.0002219,5.3845
TBPT,DEFI,0.001083,19.9843
TBPT,DEFI,0.00174,23.8956
TBPT,DEFI,0.002219,24.4764


TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,1,0.3,1,3.081,19.9391

and for reinforcements as

ET,matid,LINK180

MPDATA,EX,matid,,2e5
MPDATA,PRXY,matid,,0.3
TB,BISO,matid,1,2
TBDATA,,355,2100,,,,
R,matid,71.252, ,0


and then I combined the nodes of the link elements and solid65 using
these commands


/PREP7
ESEL,S,ENAME,,65
ESEL,A,ENAME,,180
ALLSEL,BELOW,ELEM
CEINTF,0.00001,
ALLSEL,ALL
/SOLU



and I applied a displacement of 20mm. I got a converged solution. But
as I need to see the crack patterns , I transfered the DS.DAT from WB
to ansys mechanical APDL. I can see the element solutions, But unable
to see the cracks at each step.Could you please tell me How I could
solve this
problem
Quote:
and view the cracks at different stages.
Thank you very much for your help.


Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get
a
Quote:
Quote:
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Thu Jul 17, 2014 7:07 am  Reply with quote

Peter Barrett,

As you adviced, I modelled the concrete beam as solid bodies and the
rebars as line bodies in ansys workbench. I even gave all the loading
and support condtions. By default the ansys workbench takes the
concrete body as SOLID185 and the Line bodies as BEAM188. Wat about
the contact between the concrete and the steel bars? der is no
connection developed? How do solve this problem ? How is possible to
edit the dat.ds file.If I edit so, then the file is not working in the
mechanical apdl?

Thanks and Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
p.barrett
User


Joined: 07 Oct 2013
Posts: 41

PostPosted: Thu Jul 17, 2014 7:26 am  Reply with quote

Rukmani,

If the nodes are aligned one could use the APDL command "nummrg" to tie the
rebar to the concrete.

Peter


Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rukmani Ganesan
Sent: Thursday, July 17, 2014 10:08 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Peter Barrett,

As you adviced, I modelled the concrete beam as solid bodies and the rebars
as line bodies in ansys workbench. I even gave all the loading and support
condtions. By default the ansys workbench takes the concrete body as
SOLID185 and the Line bodies as BEAM188. Wat about the contact between the
concrete and the steel bars? der is no connection developed? How do solve
this problem ? How is possible to edit the dat.ds file.If I edit so, then
the file is not working in the mechanical apdl?

Thanks and Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65
concrete element with the link 180 to model rebar or one can also
smear the rebar within the solid65 element itself (be careful to
define correct orientation and % of element area). Since Workbench
does not support this element directly one would have to use command
blocks to change the mesh from the default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block
as well with same "matid" type.

You can also access the crack plotting in APDL, but again would need
to use command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I
would recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order
elements.
Quote:
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want
the rebar to exist if creating in APDL, additional areas to load,
support, postprocess, etc.. You can use these as components in APDL
since no geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features
required in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to
use a displacement based convergence rather than force using more of an
"explicit"
Quote:
approach if you want to be able to predict the response beyond the
initial onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
rukmani.ganesan
Quote:
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I
would
Quote:
like my beam be 3d element(solid65) and the reinforcements LINK180
element.
Quote:
Is it possible that I could model? Can I see the crack pattern in the
beam
Quote:
at the time of failure in ansys workbench?I would want to gradually
increase
Quote:
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Mon Aug 04, 2014 4:19 am  Reply with quote

Hallo,

I am doing a non linear analysis of a slab in mechanical apdl. I have
applied a pressure on the top surface of the slab. I got the
deflection values.
But how do I plot the pressure against the deflection plot in the ansys apdl.
or how do get the values of the pressure applied at every subset?
Please do help me
--
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Rukmani Ganesan <rukmani.ganesan@uni-weimar.de>:

Quote:
Peter Barrett,

As you adviced, I modelled the concrete beam as solid bodies and the
rebars as line bodies in ansys workbench. I even gave all the
loading and support condtions. By default the ansys workbench takes
the concrete body as SOLID185 and the Line bodies as BEAM188. Wat
about the contact between the concrete and the steel bars? der is no
connection developed? How do solve this problem ? How is possible to
edit the dat.ds file.If I edit so, then the file is not working in
the mechanical apdl?

Thanks and Regards
Rukmani Ganesan

Bauhaus-Universitšt Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com


Zitat von Peter Barrett <barrett@caeai.com>:

Quote:
Rukmani,

Mechanical APDL (Classic) ANSYS can be used to model the solid65 concrete
element with the link 180 to model rebar or one can also smear the rebar
within the solid65 element itself (be careful to define correct orientation
and % of element area). Since Workbench does not support this element
directly one would have to use command blocks to change the mesh from the
default Solid185 to Solid65.

Example command block required for each concrete solid :

Et,matid,65
!
! would also need to add all the material data in the command block as well
with same "matid" type.

You can also access the crack plotting in APDL, but again would need to use
command blocks to create the plots in workbench.

/show,png
!
! Define view options
!
PLCRACK

While this is possible it might not be the most practical solution. I would
recommend as follows:

1) Create the geometry / mesh in WB. Make sure to use lower order elements.
Add loads, BC's etc and could add beams of rebar
2) Create a series of named selections of the edges (lines) you want the
rebar to exist if creating in APDL, additional areas to load, support,
postprocess, etc.. You can use these as components in APDL since no
geometry exists.
3) Export the Input file (DS.DAT) from WB and import into APDL
4) You can then edit this ascii file to add the concrete features required
in pre-, solution and postprocessing.
5) In regards to you pressure loading I would recommend you use many
substeps with a few iterations per substep. It often is also easier to use a
displacement based convergence rather than force using more of an "explicit"
approach if you want to be able to predict the response beyond the initial
onset of cracking.

Just an example since the ideal settings are very problem dependent:

Nsubst,500,1000,500
Neqit,5
Cnvtol,u,1e-4

Good Luck!

Peter

Peter Barrett, P.E.
CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of rukmani.ganesan
Sent: Friday, July 11, 2014 4:29 AM
To: xansys@xansys.org
Subject: [Xansys] Reinforced Concrete Beam in Ansys Workbench

Hallo,
I would like to model a reinforced concrete beam in ansys workbench. I would
like my beam be 3d element(solid65) and the reinforcements LINK180 element.
Is it possible that I could model? Can I see the crack pattern in the beam
at the time of failure in ansys workbench?I would want to gradually increase
the pressure and find the pressure at which it fails.When I do so, I get a
convergence problem.

It would be nice if someone could help me regarding this.

Rukmani Ganesan
Bauhaus-UniversitC$t Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com








~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
This email and any attachments may contain privileged or
confidential information of Computer Aided Engineering Associates.
This e-mail is intended solely for the use of the individual or
entity to which it is addressed. If you are not the intended
recipient of this e-mail, you are hereby notified that any copying,
distribution, dissemination or action taken in relation to the
contents of this e-mail and any of its attachments is strictly
prohibited and may be unlawful. If you have received this e-mail in
error, please notify the sender immediately and permanently delete
the original e-mail and destroy any copies or printouts of this
e-mail as well as any attachments.


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Mon Aug 04, 2014 5:07 am  Reply with quote

Dear Mr. Ganesan:

the time-history postprocessor (/post26) is what you need. You can
define variables containing the results at a given node or element
versus time. The commands are NSOL and ESOL. These variables are
vectors, with as many values as substeps are stored in the result file.
You can list them with the command PRVAR or plot them with the commands
PLVAR. By default they are plotted against time, which is always stored
in the first variable. You can change the abcissa in the plot by
specifying a different variable with the XVAR command.

For example, if you are interested in the displacement UZ at the node
located at the position x=10, y=5, z=0 (let us say it is the slab
center)

post26

indnode=node(10,5,0)

nvar,2,indnode,u,z,uzcenter

plvar,2 !Plot displacement versus time

The applied pressure is a boundary condition, and you should know its
time dependence.

If the pressure varies linearly with time, from p(t=0)=0 to
p(t=tmax)=pmax, you can calculate its value by multiplying the time by
the factor pmax/tmax. You can use the following command in /post26:

!Before using the commands you have

!to define the variable pmax

pmax=1000 !Change to the appropiate value

*get,tmax,vari,1,extrem,vlast !obtain the last value of time

! Define a new variable 3 with contains time*pmax/max, i.e. the applied
pressure

! It is assumed that the pressure varies linearly with time

cfact,pmax/tmax

add,3,1, , ,applied_pressure, , , pmax/tmax

!ADD, IR, IA, IB, IC, Name, --, --, FACTA, FACTB, FACTC

If the pressure has a more complicated time dependence, you could still
find a way. For example, that time dependence could be defined through a
table. In this case, you could use the command VGET to write the post26
time variable into an array, then create another array to store the
pressures at those time values, fill this array with a loop, and then
use VPUT to write the array into a post26 variable.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Universidad de Sevilla

Spain

El 04/08/2014 13:19, Rukmani Ganesan escribió:

Quote:
Hallo,

I am doing a non linear analysis of a slab in mechanical apdl. I have
applied a pressure on the top surface of the slab. I got the
deflection values.
But how do I plot the pressure against the deflection plot in the ansys apdl.
or how do get the values of the pressure applied at every subset?
Please do help me
--
Rukmani Ganesan

Bauhaus-Universität Weimar
Natural Hazards and Risks in Structural Engineeing
Tel.: +49(0)176/55446995
E-Mail: rukmani.ganesan@uni-weimar.de
rukmanig90@gmail.com

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Mon Aug 04, 2014 5:14 am  Reply with quote

I noticed a typing error. The command to enter the time-history
postprocessor is /post26

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Universidad de Sevilla

Spain

El 04/08/2014 14:07, mfernan@us.es escribió:

Quote:
Dear Mr. Ganesan:

the time-history postprocessor (/post26) is what you need. You can
define variables containing the results at a given node or element
versus time. The commands are NSOL and ESOL. These variables are
vectors, with as many values as substeps are stored in the result file.
You can list them with the command PRVAR or plot them with the commands
PLVAR. By default they are plotted against time, which is always stored
in the first variable. You can change the abcissa in the plot by
specifying a different variable with the XVAR command.

For example, if you are interested in the displacement UZ at the node
located at the position x=10, y=5, z=0 (let us say it is the slab
center)

post26

indnode=node(10,5,0)

nvar,2,indnode,u,z,uzcenter

plvar,2 !Plot displacement versus time

The applied pressure is a boundary condition, and you should know its
time dependence.

If the pressure varies linearly with time, from p(t=0)=0 to
p(t=tmax)=pmax, you can calculate its value by multiplying the time by
the factor pmax/tmax. You can use the following command in /post26:

!Before using the commands you have

!to define the variable pmax

pmax=1000 !Change to the appropiate value

*get,tmax,vari,1,extrem,vlast !obtain the last value of time

! Define a new variable 3 with contains time*pmax/max, i.e. the applied
pressure

! It is assumed that the pressure varies linearly with time

cfact,pmax/tmax

add,3,1, , ,applied_pressure, , , pmax/tmax

!ADD, IR, IA, IB, IC, Name, --, --, FACTA, FACTB, FACTC

If the pressure has a more complicated time dependence, you could still
find a way. For example, that time dependence could be defined through a
table. In this case, you could use the command VGET to write the post26
time variable into an array, then create another array to store the
pressures at those time values, fill this array with a loop, and then
use VPUT to write the array into a post26 variable.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Universidad de Sevilla

Spain

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rukmani.ganesan
User


Joined: 10 Jul 2014
Posts: 13

PostPosted: Mon Aug 04, 2014 5:55 am  Reply with quote

Dear Mr.Jose

thank you very much for your reply.

I am not so well familiar with the coammands in ansys apdl. I am using the GUI.
As you advised, I could get the deflections at a node at every subset in the centre of the slab.

I am doing an non linear analysis of a reinforced concrete slab. I had applied a pressure on the top AREA of the slab .
But how do I get the values of the applied pressure at every subset..For every substep a pressure would be applied. And how will get to know these values?

for example. I applied a pressure of 0.2 MPa on the surface area of the slab.
and in the solution controls, I have given minmum and intial subsets as 150 and maximum as 500. Depending on subsets values, the load gets slowly incremented on the slap right?
How can I get the list of these pressure values at every subset ? I dont want it specifically on a node. I want to know overall how the pressure had been divided and applied.

Do you think its possible?
Please do help me.

Thanks and Regards
Rukmani
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron