XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Creating inclined boundary conditions in APDL
 
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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Wed Jul 09, 2014 1:46 am  Reply with quote

Hello everyone,

I am modelling a shell surface in APDL. Shell structural performance is optimal when the support reaction is exactly tangential to the shell surface. The current boundary conditions have been applied by picking the edge line of shell and constraining UZ only. Could anyone help me to define the boundary conditions as shown in image 'support system_reqd.JPG' ?

See images at following Dropbox link;
https://www.dropbox.com/sh/aznbqem251sfy96/AADpjczPrjzD_TaIFYEsXq8ra

Best regards,
Sushant Goel
MSc student, Uni Stuttgart
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Wed Jul 09, 2014 3:18 am  Reply with quote

Dear Mr. Goel,

you can rotate the nodal system of coordinates of all the nodes on the
support. Check the commands nmodif,nrotat,nang, nora.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 09/07/2014 10:46, sushant.goel escribió:

Quote:
Hello everyone,

I am modelling a shell surface in APDL. Shell structural performance is optimal when the support reaction is exactly tangential to the shell surface. The current boundary conditions have been applied by picking the edge line of shell and constraining UZ only. Could anyone help me to define the boundary conditions as shown in image 'support system_reqd.JPG' ?

See images at following Dropbox link;
https://www.dropbox.com/sh/aznbqem251sfy96/AADpjczPrjzD_TaIFYEsXq8ra [1]

Best regards,
Sushant Goel
MSc student, Uni Stuttgart


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [4] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [5] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] https://www.dropbox.com/sh/aznbqem251sfy96/AADpjczPrjzD_TaIFYEsXq8ra
[2] http://www.mail2forum.com
[3] http://xansys.org/forum/viewtopic.php?p=94768#94768
[4] http://www.xansys.org/forum
[5] http://www.padtinc.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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Wed Jul 23, 2014 1:18 am  Reply with quote

Quote:
Dear Mr. Goel,

you can rotate the nodal system of coordinates of all the nodes on the
support. Check the commands nmodif,nrotat,nang, nora.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain


Dear Mr Galan,

Thank you for the reply. Yes you were right about rotating the nodal system of coordinates of all nodes on the support. I am rotating them in the direction of surface normal of the immediate element attached to that boundary node. [Preprocessor> Modeling> Move/Modify> Rotate node CS> To Surf Norm]

But the issue now is that I have to click on each and every boundary node in the FE model (and I have to repeat this in 12 FE models) and then assign a neighboring element for surface normal. Can I somehow extract the boundary nodes and neighboring elements list to define a batch file in APDL?

Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Jul 24, 2014 8:17 am  Reply with quote

Dear Mr. Goel:

it seems that you are using the command NORA that rotates the nodal
coordinate systems to the surface normal. Is this correct?

If you see the help on that command, you can see it rotates all the
selected nodes. In addition, you can specify more than one area (in
fact, ALL the selected areas, that can be previously selected with the
command ASEL). You do not need to apply the command for each individual
node.

I would like to highlight a paragraph of the help:

"In case multiple areas are selected, there could be conflicts at the
boundaries. If a node belongs to two areas that have a different normal,
its nodal coordinate system will be rotated to the area normal with the
lowest number."

You could first select all the nodes that you want to rotate. There are
several ways to do so, depending on your geometry. For example, if they
all belonged to the one line, you would first select the line (with the
command LSEL,S,), and then select nodes attached to line (NSLL,S). For
example, if they were all located at Z=0, you could select them with the
command NSEL,S,LOC,Z,0

Once all the edge nodes are selected, you have to select all the areas
that contain the nodes. You could try first ASEL,ALL.

You could try these commands and see if they work for you.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. 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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Mon Aug 04, 2014 2:46 am  Reply with quote

Quote:
Dear Mr. Goel:

it seems that you are using the command NORA that rotates the nodal
coordinate systems to the surface normal. Is this correct?

If you see the help on that command, you can see it rotates all the
selected nodes. In addition, you can specify more than one area (in
fact, ALL the selected areas, that can be previously selected with the
command ASEL). You do not need to apply the command for each individual
node.

I would like to highlight a paragraph of the help:

"In case multiple areas are selected, there could be conflicts at the
boundaries. If a node belongs to two areas that have a different normal,
its nodal coordinate system will be rotated to the area normal with the
lowest number."

You could first select all the nodes that you want to rotate. There are
several ways to do so, depending on your geometry. For example, if they
all belonged to the one line, you would first select the line (with the
command LSEL,S,), and then select nodes attached to line (NSLL,S). For
example, if they were all located at Z=0, you could select them with the
command NSEL,S,LOC,Z,0

Once all the edge nodes are selected, you have to select all the areas
that contain the nodes. You could try first ASEL,ALL.

You could try these commands and see if they work for you.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain


Dear Mr Galan,

Thank you for the reply. I am using the following commands for the required support system.

/TITLE,local_7_G
/PREP7
ET,1,SHELL181
SECTYPE,,SHELL
SECDATA,10
MP,EX,1,70000
MP,PRXY,1,0.22
MP,DENS,1,2.5e-6
LOCAL,12,2
ESYS,12
AESIZE,ALL,50
AMESH,ALL
LSEL,S,LOC,Z,0
NORL,ALL,ALL,-1
FINISH
/SOLU
ALLSEL
ANTYPE,STATIC
NSEL,S,LOC,Z,0
D,ALL,UX,0
ALLSEL
ACEL,,,9.81
SOLVE
FINISH

How can I verify in APDL that this script is generating the supports which are exactly tangential? I want to do this because after solving, I am not getting the expected deflection results.

Best regards,
Sushant Goel
MSc Uni Stuttgart
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Mon Aug 04, 2014 5:35 am  Reply with quote

Dear Mr. Goel:

to check if your nodes are properly rotated, you can show the nodal
coordinate system in your plots. This is done with the command

/PSYMB,ndir,1

Then, use nplot or eplot and visually check the orientation of the

I think that the problem may be that you are not aware of the definition
of spherical coordinate systems in ansys. You can find the information
in the appropiate section of ansys manual, where it describes the
spherical and cylindrical coordinate systems. Here I send you the link
(ansys 15 help): help/ans_mod/Hlp_G_MOD3_2.html

You are using an spherical system of coordinates (local,12,2). That
means that coordinates (X,Y,Z) are respectively (R,theta,phi), where
theta is the circunferential direction and phi is the meridional
direction defined with respect to the plane Z=0.

In your supports you are restraining the UX displacement (d,all,ux,0),
which in a spherical coordinate system means that you are restraining
the radial displacement (UR). That is not what you intended to do. You
wanted to eliminate the local shell bending at the supports, by
constraining the meridional (tangential) displacements only. Therefore,
in your spherical coordinate system you should restrain UZ.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

University of Sevilla

Spain

Quote:
Dear Mr Galan,

Thank you for the reply. I am using the following commands for the required support system.

/TITLE,local_7_G
/PREP7
ET,1,SHELL181
SECTYPE,,SHELL
SECDATA,10
MP,EX,1,70000
MP,PRXY,1,0.22
MP,DENS,1,2.5e-6
LOCAL,12,2
ESYS,12
AESIZE,ALL,50
AMESH,ALL
LSEL,S,LOC,Z,0
NORL,ALL,ALL,-1
FINISH
/SOLU
ALLSEL
ANTYPE,STATIC
NSEL,S,LOC,Z,0
D,ALL,UX,0
ALLSEL
ACEL,,,9.81
SOLVE
FINISH

How can I verify in APDL that this script is generating the supports which are exactly tangential? I want to do this because after solving, I am not getting the expected deflection results.

Best regards,
Sushant Goel
MSc Uni Stuttgart

+-------------------------------------------------------------+
| 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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Tue Aug 05, 2014 7:18 am  Reply with quote

Quote:
Dear Mr. Goel:

to check if your nodes are properly rotated, you can show the nodal
coordinate system in your plots. This is done with the command

/PSYMB,ndir,1

Then, use nplot or eplot and visually check the orientation of the

I think that the problem may be that you are not aware of the definition
of spherical coordinate systems in ansys. You can find the information
in the appropiate section of ansys manual, where it describes the
spherical and cylindrical coordinate systems. Here I send you the link
(ansys 15 help): help/ans_mod/Hlp_G_MOD3_2.html

You are using an spherical system of coordinates (local,12,2). That
means that coordinates (X,Y,Z) are respectively (R,theta,phi), where
theta is the circunferential direction and phi is the meridional
direction defined with respect to the plane Z=0.

In your supports you are restraining the UX displacement (d,all,ux,0),
which in a spherical coordinate system means that you are restraining
the radial displacement (UR). That is not what you intended to do. You
wanted to eliminate the local shell bending at the supports, by
constraining the meridional (tangential) displacements only. Therefore,
in your spherical coordinate system you should restrain UZ.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

University of Sevilla

Spain


Dear Mr Galan,

Thank you for the reply and help link. I defined the spherical coordinate system for aligning the element coordinates in hoop and meridian direction. This makes it easy to read hoop and meridian forces and stresses.

https://www.dropbox.com/s/fuvecyucyvpeeff/coordinate.PNG

In the above image, the nodal coordinates at base of dome are shown. Even after using spherical coordinate system, (d,all,uz,0) doesn't constrain the meridian displacement. That's why I am using (d,all,ux,0). Result is shown in image below.

https://www.dropbox.com/s/l8u51dpslhtoxe4/s3.png

Does this mean that the nodal coordinate system is unaffected by coordinate system changes?

Another query is regarding the unrealistic deflections (818 meters) as shown in images below;
https://www.dropbox.com/s/g4kl52c1ptz1orj/deflection.PNG
https://www.dropbox.com/s/atlyb0se9mv2q5g/shape.PNG

Do you have any idea why this is happening?

Best regards,
Sushant
MSc Uni Stuttgart

/TITLE,local_7_G
/PREP7
ET,1,SHELL181
SECTYPE,,SHELL
SECDATA,10
MP,EX,1,70000
MP,PRXY,1,0.22
MP,DENS,1,2.5e-9
LOCAL,12,2
ESYS,12
AESIZE,ALL,50
AMESH,ALL
LSEL,S,LOC,Z,0
NORL,ALL,ALL,-1
FINISH
/SOLU
ALLSEL
ANTYPE,STATIC
NSEL,S,LOC,Z,0
D,ALL,UX,0
ALLSEL
ACEL,,,9810
SOLVE
FINISH
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 05, 2014 8:51 am  Reply with quote

Dear Mr. Goel:

I apologize, your boundary condition was right. My mistake.

You rotate the element coordinate system into the global spherical
coordinate system with the command Esys,12. Those orientation are just
as I told you.

On the other hand, your nodal coordinate system is not rotated to
coincide with the global spherical system. You would obtain that
rotation if you used the command NROTAT. You could try it and see:

nsel,s,loc,z,0

nrotat,all

/psymb,ndir,1

eplot

You are using the command NORL to rotate the nodal coordinate system. If
you look at the help of the command, it says that it "rotates the X-axis
of the nodal coordinate perpendicular to the line normal". That is, in
your case, the meridional direction, as it is clear from the figures
that you sent. The boundary condition that you were applying was
correct.

If you only use that boundary condition, your structure is still a
mechanism. You should restrain it more. Have you noticed that your
displacement results do not have symmetry of revolution around the
global Z axis? It seems that the structure is rotating. That may be
rigid body motion.

Have you checked your units? It seems that you are using N for forces,
mm for distances, and kg for mass. Is this correct? If so, you are using
E=20000 N/mm^2=20 GPa, which is a reasonable value for concrete. The
acceleration of gravity is also correct, g=9.81 m/s^2=9810 mm/s^2. But
the density seems too small: for concrete is about rho=2500 kg/m^3=2.5
e-6 kg /m, while in your input file it is 1000 times smaller. On the
other hand, this is not the case of your problem.

Your shell is under compression, and it may buckle. Do you have large
deflection (NLGEOM,on) or prestressing effect (PSTRES,ON) activated?

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. 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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Tue Aug 05, 2014 9:11 am  Reply with quote

Quote:
Dear Mr. Goel:

I apologize, your boundary condition was right. My mistake.

You rotate the element coordinate system into the global spherical
coordinate system with the command Esys,12. Those orientation are just
as I told you.

On the other hand, your nodal coordinate system is not rotated to
coincide with the global spherical system. You would obtain that
rotation if you used the command NROTAT. You could try it and see:

nsel,s,loc,z,0

nrotat,all

/psymb,ndir,1

eplot

You are using the command NORL to rotate the nodal coordinate system. If
you look at the help of the command, it says that it "rotates the X-axis
of the nodal coordinate perpendicular to the line normal". That is, in
your case, the meridional direction, as it is clear from the figures
that you sent. The boundary condition that you were applying was
correct.

If you only use that boundary condition, your structure is still a
mechanism. You should restrain it more. Have you noticed that your
displacement results do not have symmetry of revolution around the
global Z axis? It seems that the structure is rotating. That may be
rigid body motion.

Have you checked your units? It seems that you are using N for forces,
mm for distances, and kg for mass. Is this correct? If so, you are using
E=20000 N/mm^2=20 GPa, which is a reasonable value for concrete. The
acceleration of gravity is also correct, g=9.81 m/s^2=9810 mm/s^2. But
the density seems too small: for concrete is about rho=2500 kg/m^3=2.5
e-6 kg /m, while in your input file it is 1000 times smaller. On the
other hand, this is not the case of your problem.

Your shell is under compression, and it may buckle. Do you have large
deflection (NLGEOM,on) or prestressing effect (PSTRES,ON) activated?

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain


Dear Mr Galan,

No problem sir. Yes, I will try NROTAT in order to orient the nodal coordinate system to global spherical coordinate system.

I was also confused with the unsymmetrical (about global z) displacement results. I will add additional constraints to the dome edge by fixing theta (in spherical system now) for some nodes.

https://www.dropbox.com/s/bvjhnuo2byhdbo1/ansys%20units.PNG

Please see the table given in the link above. I have used this to maintain unit consistency.

The values I am using are;
SHELL181, 10 mm thick glass
E= 70000 N/mm2 = 70 GPa
g=9810 mm/s2
density= 2500 kg/m3 = 2.5e-9 tonne/mm3

The output units would be -
Moment per unit length- Nmm/mm
Stress - N/mm2
Deflection - mm

Please correct me if there is some discrepancy with units.

NLGEOM and PSTRES have not been used. I will run the simulation again with added constraints and share the results.

Best regards,
Sushant
MSc Uni Stuttgart
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 05, 2014 9:33 am  Reply with quote

Dear Mr. Goel,

You are right, your units are consistent.

Those constrains in theta direction are a good idea, and they will stop
the rotation around the global Z axis.

You can check if all the rigid body modes are constrained by calculating
the natural frequencies of your structure. Rigid body modes show up as
zeroes. By plotting their deformed shape you also get an idea on how to
constrain them.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. 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
sushant.goel
User


Joined: 08 May 2014
Posts: 66

PostPosted: Wed Aug 06, 2014 12:19 am  Reply with quote

Quote:
Dear Mr. Goel,

You are right, your units are consistent.

Those constrains in theta direction are a good idea, and they will stop
the rotation around the global Z axis.

You can check if all the rigid body modes are constrained by calculating
the natural frequencies of your structure. Rigid body modes show up as
zeroes. By plotting their deformed shape you also get an idea on how to
constrain them.

Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain


Dear Mr Galan,

Thank you once again.

Best regards,
Sushant Goel
Uni Stuttgart
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