XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
NODE values in tables
 
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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Tue Jun 17, 2014 3:21 am  Reply with quote

Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to
go all the elements one by one, then get the NODE numbers of each element,
keep them in the table/array and then get for instance information about the
temperatures in nodes. But I am having difficulties of realizing this and writing
an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material properties of each element of
the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jun 17, 2014 4:52 am  Reply with quote

Dear Mr. Martirosyan,

In ansys the material properties can be defined at several temperatures
(see commands TBTEMP and TBDATA). At each integration points, ansys uses
the temperature at that point to interpolate the material properties.
This interpolation is the same as in TABLE arrays. You may consider if
defining temperature-dependent material properties is applicable to your
problem.

Please, check the following section of the ansys manual:

Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining
Material Properties

Theory Reference | Chapter 13. Element Tools | 13.4.
Temperature-Dependent Material Properties

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 12:21, razmik.martirosyan escribió:

Quote:
Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to
go all the elements one by one, then get the NODE numbers of each element,
keep them in the table/array and then get for instance information about the
temperatures in nodes. But I am having difficulties of realizing this and writing
an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material properties of each element of
the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona

+-------------------------------------------------------------+
| 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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Tue Jun 17, 2014 5:24 am  Reply with quote

Dear Mr. GAlan,

Thank you for your answer, but the problem is that the properties does not
only depend on temperatures therefore they should be defined as functions of other
things also(such as humidity, etc.), so in this case I am not having possibility
to use these commands.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Cataluña

jose.galan wrote:
Dear Mr. Martirosyan,

In ansys the material properties can be defined at several temperatures
(see commands TBTEMP and TBDATA). At each integration points, ansys uses
the temperature at that point to interpolate the material properties.
This interpolation is the same as in TABLE arrays. You may consider if
defining temperature-dependent material properties is applicable to your
problem.

Please, check the following section of the ansys manual:

Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining
Material Properties

Theory Reference | Chapter 13. Element Tools | 13.4.
Temperature-Dependent Material Properties

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 12:21, razmik.martirosyan escribió:

Quote:
Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to
go all the elements one by one, then get the NODE numbers of each element,
keep them in the table/array and then get for instance information about the
temperatures in nodes. But I am having difficulties of realizing this and writing
an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material properties of each element of
the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona

+-------------------------------------------------------------+
| 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
rick.fischer
User


Joined: 31 Aug 2011
Posts: 198

PostPosted: Tue Jun 17, 2014 5:46 am  Reply with quote

If I understand this correctly, you need to get nodal data sorted to elements. One way to do this is with the *voper,,,gath command. I don't know anything about your model or concrete curing, but lets say you have 4-node tet elements and your material properties are changing as a function of temperature, and you need the average nodal temp for the element. It will look something like this:

ecount=elmiqr(0,14)
ncount=ndinqr(0,14)

*dim,ndata,,ncount,4
*dim,edata,,ecount,5
*dim,tdata,,ecount,4

*dim,spud,,4
spud(1)=.25,.25,.25,.25

*vget,edata(1,1),elem,1,node,1
*vget,edata(1,2),elem,2,node,2
*vget,edata(1,3),elem,3,node,3
*vget,edata(1,4),elem,4,node,4

*vget,ndata,node,1,temp

*voper,tdata(1,1),ndata(1,1),gath,edata(1,1)
*voper,tdata(1,2),ndata(1,1),gath,edata(1,2)
*voper,tdata(1,3),ndata(1,1),gath,edata(1,3)
*voper,tdata(1,4),ndata(1,1),gath,edata(1,4)

*moper,edata(1,5),tdata(1,1),mult,spud(1)

Ndata will hold the nodal temps, edata will hold the node numbers at the four corners of the tets and tdata will hold the elemental corner temps. Edata and ndata are filled with *vget commands, and tdata is filled by gathering nodal temps from ndata per the order given in edata. The final *moper will produce the average of four nodal temps in the fifth column of edata. This last bit works if all the elements have four nodes. If you have a mesh of all bricks, first you'll need bigger arrays because you have more nodes. Then *dim,spud,,8 and spud(1)=.125,125,.125,.125,.125,.125,.125,.125. If the mesh is mixed, it gets a bit messy to get the average temp. You would have to set spud to all 1's, then look at edata(1,5) and see if it is a zero. If so, it's a tet and you divide that row by 4, if not, it's a brick and divide that row by 8. There are a couple of ways to do this. One would be:

*vfill edata(1,9),ramp,4,0
*voper,edata(1,10),edata(1,5),ne,0
*vmask,edata(1,10)
*voper,edata(1,9),edata(1,9),mult,2
*moper,edata(1,11),tdata(1,1),mult,spud(1)
*voper,edata(1,12),edata(1,11),div,edata(1,9)

Hope this helps.

Rick Fischer
Principal Engineer
Argonne National Laboratory

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of razmik.martirosyan
Sent: Tuesday, June 17, 2014 5:21 AM
To: xansys@xansys.org
Subject: [Xansys] NODE values in tables

Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to go all the elements one by one, then get the NODE numbers of each element, keep them in the table/array and then get for instance information about the temperatures in nodes. But I am having difficulties of realizing this and writing an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material properties of each element of the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona






+-------------------------------------------------------------+
| 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)
_________________
Rick Fischer
Principal Engineer
Argonne National Laboratory
Back to top
View user's profile Send private message Send e-mail
rick.fischer
User


Joined: 31 Aug 2011
Posts: 198

PostPosted: Tue Jun 17, 2014 5:49 am  Reply with quote

But you can still use temperature to vary the material properties. Program some APDL to give you dummy temps which you apply as a structural load. It will change the material properties. Just pretend its humidity.

Rick Fischer
Principal Engineer
Argonne National Laboratory


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of razmik.martirosyan
Sent: Tuesday, June 17, 2014 7:25 AM
To: xansys@xansys.org
Subject: Re: [Xansys] NODE values in tables

Dear Mr. GAlan,

Thank you for your answer, but the problem is that the properties does not only depend on temperatures therefore they should be defined as functions of other things also(such as humidity, etc.), so in this case I am not having possibility to use these commands.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Cataluña


jose.galan wrote:
Quote:
Dear Mr. Martirosyan,

In ansys the material properties can be defined at several
temperatures (see commands TBTEMP and TBDATA). At each integration
points, ansys uses the temperature at that point to interpolate the material properties.
This interpolation is the same as in TABLE arrays. You may consider if
defining temperature-dependent material properties is applicable to
your problem.

Please, check the following section of the ansys manual:

Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining
Material Properties

Theory Reference | Chapter 13. Element Tools | 13.4.
Temperature-Dependent Material Properties

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 12:21, razmik.martirosyan escribió:


Quote:
Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to go
all the elements one by one, then get the NODE numbers of each
element, keep them in the table/array and then get for instance
information about the temperatures in nodes. But I am having
difficulties of realizing this and writing an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material
properties of each element of the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona


+-------------------------------------------------------------+
| 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)
_________________
Rick Fischer
Principal Engineer
Argonne National Laboratory
Back to top
View user's profile Send private message Send e-mail
james.kosloski
User


Joined: 11 Mar 2011
Posts: 56

PostPosted: Tue Jun 17, 2014 5:54 am  Reply with quote

Take a look at the TBFIELD command with a user defined field variable.

________________________________


James J. Kosloski
Senior Engineering Manager

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

P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
razmik.martirosyan
Sent: Tuesday, June 17, 2014 8:25 AM
To: xansys@xansys.org
Subject: Re: [Xansys] NODE values in tables

Dear Mr. GAlan,

Thank you for your answer, but the problem is that the properties does not
only depend on temperatures therefore they should be defined as functions of
other things also(such as humidity, etc.), so in this case I am not having
possibility to use these commands.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de CataluC1a


jose.galan wrote:
Quote:
Dear Mr. Martirosyan,

In ansys the material properties can be defined at several
temperatures (see commands TBTEMP and TBDATA). At each integration
points, ansys uses the temperature at that point to interpolate the
material properties.
Quote:
This interpolation is the same as in TABLE arrays. You may consider if
defining temperature-dependent material properties is applicable to
your problem.

Please, check the following section of the ansys manual:

Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining
Material Properties

Theory Reference | Chapter 13. Element Tools | 13.4.
Temperature-Dependent Material Properties

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 12:21, razmik.martirosyan escribiC3:


Quote:
Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening
concrete, and while doing transient analysis, after meshing,in each step I
have to get the node values of each element and then use them to obtain the
properties of the material in the next step.
Quote:
Quote:

As I know ANSYS allows using of tables/arrays so I am thinking to go
all the elements one by one, then get the NODE numbers of each
element, keep them in the table/array and then get for instance
information about the temperatures in nodes. But I am having
difficulties of realizing this and writing an appropriate function.
Could you please help me with this issue?
Quote:
Quote:

Also, if you have information about how to change material
properties of each element of the mesh between steps, depending on the
last step results, please let me know.
Quote:
Quote:

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona


+-------------------------------------------------------------+
| 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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Jun 17, 2014 10:29 am  Reply with quote

You could try mpchg.

You may also consider creating a function in fortran with your own
material model through User Programmable Features. For this latter
option, you should check the Programmer's Manual for Mechanical APDL

http://orange.engr.ucdavis.edu/Documentation12.1/121/ans_prog.pdf

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 14:54, James J. Kosloski escribió:

Quote:
Take a look at the TBFIELD command with a user defined field variable.

________________________________

James J. Kosloski
Senior Engineering Manager

CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com [1]

P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
razmik.martirosyan
Sent: Tuesday, June 17, 2014 8:25 AM
To: xansys@xansys.orgSubject: Re: [Xansys] NODE values in tables

Dear Mr. GAlan,

Thank you for your answer, but the problem is that the properties does not
only depend on temperatures therefore they should be defined as functions of
other things also(such as humidity, etc.), so in this case I am not having
possibility to use these commands.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de CataluC1a

jose.galan wrote:

Quote:
Dear Mr. Martirosyan, In ansys the material properties can be defined at several temperatures (see commands TBTEMP and TBDATA). At each integration points, ansys uses the temperature at that point to interpolate the

material properties.
This interpolation is the same as in TABLE arrays. You may consider if defining temperature-dependent material properties is applicable to your problem. Please, check the following section of the ansys manual: Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining Material Properties Theory Reference | Chapter 13. Element Tools | 13.4. Temperature-Dependent Material Properties Best regards, Jose M. Galan Asst.Prof. Constr. Eng. Dpt. Univ. Sevilla Spain El 17/06/2014 12:21, razmik.martirosyan escribiC3: Hello everyone, By Using ANSYS APDL I am trying to simulate the behaviour of hardening

concrete, and while doing transient analysis, after meshing,in each step
I
have to get the node values of each element and then use them to obtain
the
properties of the material in the next step.

Quote:
Quote:
As I know ANSYS allows using of tables/arrays so I am thinking to go all the elements one by one, then get the NODE numbers of each element, keep them in the table/array and then get for instance information about the temperatures in nodes. But I am having difficulties of realizing this and writing an appropriate function.

Could you please help me with this issue?

Quote:
Quote:
Also, if you have information about how to change material properties of each element of the mesh between steps, depending on the

last step results, please let me know.

Quote:
Quote:
Best Regards Razmik Martirosyan Universitat Polytechnica de Barcelona
+-------------------------------------------------------------+ | XANSYS web - www.xansys.org/forum [2] | | The Online Community for users of ANSYS, Inc. Software | | Hosted by PADT - www.padtinc.com [3] | | Send administrative requests to xansys-mod@tynecomp.co.uk | +-------------------------------------------------------------+ Post generated using Mail2Forum (http://www.mail2forum.com [4])


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
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 [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



Links:
------
[1] http://www.caeai.com
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
[4] http://www.mail2forum.com
[5] http://xansys.org/forum/viewtopic.php?p=94524#94524
+-------------------------------------------------------------+
| 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
paul.bales
User


Joined: 01 Jun 2009
Posts: 7

PostPosted: Tue Jun 17, 2014 11:32 am  Reply with quote

Thanks. I just ended up defining it for each bolt separately, and it seemed to work OK.

I would like to be able to plot the force in each bolt as a function of time. I think you said that I'd have to put some kind of force monitor in my model when I run it in order to get that information, correct? I can't just do it in the post-processor? Can you point me towards the keyword necessary to accomplish this?

Thanks,
Paul

-----------------------------------
Paul Bales
Senior Engineering Analyst
USEC
(865) 425-6581


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: Tuesday, June 17, 2014 1:30 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] NODE values in tables



You could try mpchg.

You may also consider creating a function in fortran with your own material model through User Programmable Features. For this latter option, you should check the Programmer's Manual for Mechanical APDL

http://orange.engr.ucdavis.edu/Documentation12.1/121/ans_prog.pdf

Best regards,

Jose M. Galan

Asst.Prof.

Constr. Eng. Dpt.

Univ. Sevilla

Spain

El 17/06/2014 14:54, James J. Kosloski escribió:

Quote:
Take a look at the TBFIELD command with a user defined field variable.

________________________________

James J. Kosloski
Senior Engineering Manager

CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com
[1]

P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
razmik.martirosyan
Sent: Tuesday, June 17, 2014 8:25 AM
To: xansys@xansys.orgSubject: Re: [Xansys] NODE values in tables

Dear Mr. GAlan,

Thank you for your answer, but the problem is that the properties does
not only depend on temperatures therefore they should be defined as
functions of other things also(such as humidity, etc.), so in this
case I am not having possibility to use these commands.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de CataluC1a

jose.galan wrote:

Quote:
Dear Mr. Martirosyan, In ansys the material properties can be defined
at several temperatures (see commands TBTEMP and TBDATA). At each
integration points, ansys uses the temperature at that point to
interpolate the

material properties.
This interpolation is the same as in TABLE arrays. You may consider if
defining temperature-dependent material properties is applicable to
your problem. Please, check the following section of the ansys manual:
Basic Guide | Chapter 1. Getting Started with ANSYS | 1.1.4. Defining
Material Properties Theory Reference | Chapter 13. Element Tools |
13.4. Temperature-Dependent Material Properties Best regards, Jose M.
Galan Asst.Prof. Constr. Eng. Dpt. Univ. Sevilla Spain El 17/06/2014
12:21, razmik.martirosyan escribiC3: Hello everyone, By Using ANSYS
APDL I am trying to simulate the behaviour of hardening

concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

Quote:
Quote:
As I know ANSYS allows using of tables/arrays so I am thinking to go all the elements one by one, then get the NODE numbers of each element, keep them in the table/array and then get for instance information about the temperatures in nodes. But I am having difficulties of realizing this and writing an appropriate function.

Could you please help me with this issue?

Quote:
Quote:
Also, if you have information about how to change material properties
of each element of the mesh between steps, depending on the

last step results, please let me know.

Quote:
Quote:
Best Regards Razmik Martirosyan Universitat Polytechnica de Barcelona
+-------------------------------------------------------------+ | XANS
+-------------------------------------------------------------+ | YS
+-------------------------------------------------------------+ | web
+-------------------------------------------------------------+ | -
+-------------------------------------------------------------+ | www.
+-------------------------------------------------------------+ | xans
+-------------------------------------------------------------+ | ys.o
+-------------------------------------------------------------+ | rg/f
+-------------------------------------------------------------+ | orum
+-------------------------------------------------------------+ | [2]
+-------------------------------------------------------------+ | | |
+-------------------------------------------------------------+ | The
+-------------------------------------------------------------+ | Onli
+-------------------------------------------------------------+ | ne
+-------------------------------------------------------------+ | Comm
+-------------------------------------------------------------+ | unit
+-------------------------------------------------------------+ | y
+-------------------------------------------------------------+ | for
+-------------------------------------------------------------+ | user
+-------------------------------------------------------------+ | s of
+-------------------------------------------------------------+ | ANSY
+-------------------------------------------------------------+ | S,
+-------------------------------------------------------------+ | Inc.
+-------------------------------------------------------------+ | Soft
+-------------------------------------------------------------+ | ware
+-------------------------------------------------------------+ | | |
+-------------------------------------------------------------+ | Host
+-------------------------------------------------------------+ | ed
+-------------------------------------------------------------+ | by
+-------------------------------------------------------------+ | PADT
+-------------------------------------------------------------+ | -
+-------------------------------------------------------------+ | www.
+-------------------------------------------------------------+ | padt
+-------------------------------------------------------------+ | inc.
+-------------------------------------------------------------+ | com
+-------------------------------------------------------------+ | [3]
+-------------------------------------------------------------+ | | |
+-------------------------------------------------------------+ | Send
+-------------------------------------------------------------+ | admi
+-------------------------------------------------------------+ | nist
+-------------------------------------------------------------+ | rati
+-------------------------------------------------------------+ | ve
+-------------------------------------------------------------+ | requ
+-------------------------------------------------------------+ | ests
+-------------------------------------------------------------+ | to
+-------------------------------------------------------------+ | xans
+-------------------------------------------------------------+ | ys-m
+-------------------------------------------------------------+ | od@t
+-------------------------------------------------------------+ | ynec
+-------------------------------------------------------------+ | omp.
+-------------------------------------------------------------+ | co.u
+-------------------------------------------------------------+ | k |
+-------------------------------------------------------------+ | +---
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | ----
+-------------------------------------------------------------+ | --+
+-------------------------------------------------------------+ | Post
+-------------------------------------------------------------+ | gene
+-------------------------------------------------------------+ | rate
+-------------------------------------------------------------+ | d
+-------------------------------------------------------------+ | usin
+-------------------------------------------------------------+ | g
+-------------------------------------------------------------+ | Mail
+-------------------------------------------------------------+ | 2For
+-------------------------------------------------------------+ | um
+-------------------------------------------------------------+ | (htt
+-------------------------------------------------------------+ | p://
+-------------------------------------------------------------+ | www.
+-------------------------------------------------------------+ | mail
+-------------------------------------------------------------+ | 2for
+-------------------------------------------------------------+ | um.c
+-------------------------------------------------------------+ | om
+-------------------------------------------------------------+ | [4])


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
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 [2] | The Online Community for users
| of ANSYS, Inc. Software | Hosted by PADT - www.padtinc.com [3] | Send
| administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+



Links:
------
[1] http://www.caeai.com
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
[4] http://www.mail2forum.com
[5] http://xansys.org/forum/viewtopic.php?p=94524#94524
+-------------------------------------------------------------+
| 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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Wed Jun 18, 2014 2:56 am  Reply with quote

Dear Mr. Fischer,

Thank you! Your code helped a lot, that is what I Wanted, although one small
question left.

As I told I want to change the parameters of material for each element of the mesh,
between time steps, and I am not able to define them before analysis, as they may
depend on the results of the last step, therefore I think I might not use the command
MPCHG.

Any suggestion how to handle these procedures?

Best Regards
Razmik Martirosyan
Universitat Polytecnica de Cataluña

rick.fischer wrote:
If I understand this correctly, you need to get nodal data sorted to elements. One way to do this is with the *voper,,,gath command. I don't know anything about your model or concrete curing, but lets say you have 4-node tet elements and your material properties are changing as a function of temperature, and you need the average nodal temp for the element. It will look something like this:

ecount=elmiqr(0,14)
ncount=ndinqr(0,14)

*dim,ndata,,ncount,4
*dim,edata,,ecount,5
*dim,tdata,,ecount,4

*dim,spud,,4
spud(1)=.25,.25,.25,.25

*vget,edata(1,1),elem,1,node,1
*vget,edata(1,2),elem,2,node,2
*vget,edata(1,3),elem,3,node,3
*vget,edata(1,4),elem,4,node,4

*vget,ndata,node,1,temp

*voper,tdata(1,1),ndata(1,1),gath,edata(1,1)
*voper,tdata(1,2),ndata(1,1),gath,edata(1,2)
*voper,tdata(1,3),ndata(1,1),gath,edata(1,3)
*voper,tdata(1,4),ndata(1,1),gath,edata(1,4)

*moper,edata(1,5),tdata(1,1),mult,spud(1)

Ndata will hold the nodal temps, edata will hold the node numbers at the four corners of the tets and tdata will hold the elemental corner temps. Edata and ndata are filled with *vget commands, and tdata is filled by gathering nodal temps from ndata per the order given in edata. The final *moper will produce the average of four nodal temps in the fifth column of edata. This last bit works if all the elements have four nodes. If you have a mesh of all bricks, first you'll need bigger arrays because you have more nodes. Then *dim,spud,,8 and spud(1)=.125,125,.125,.125,.125,.125,.125,.125. If the mesh is mixed, it gets a bit messy to get the average temp. You would have to set spud to all 1's, then look at edata(1,5) and see if it is a zero. If so, it's a tet and you divide that row by 4, if not, it's a brick and divide that row by 8. There are a couple of ways to do this. One would be:

*vfill edata(1,9),ramp,4,0
*voper,edata(1,10),edata(1,5),ne,0
*vmask,edata(1,10)
*voper,edata(1,9),edata(1,9),mult,2
*moper,edata(1,11),tdata(1,1),mult,spud(1)
*voper,edata(1,12),edata(1,11),div,edata(1,9)

Hope this helps.

Rick Fischer
Principal Engineer
Argonne National Laboratory

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of razmik.martirosyan
Sent: Tuesday, June 17, 2014 5:21 AM
To: xansys@xansys.org
Subject: [Xansys] NODE values in tables

Hello everyone,

By Using ANSYS APDL I am trying to simulate the behaviour of hardening concrete, and while doing transient analysis, after meshing,in each step I have to get the node values of each element and then use them to obtain the properties of the material in the next step.

As I know ANSYS allows using of tables/arrays so I am thinking to go all the elements one by one, then get the NODE numbers of each element, keep them in the table/array and then get for instance information about the temperatures in nodes. But I am having difficulties of realizing this and writing an appropriate function. Could you please help me with this issue?

Also, if you have information about how to change material properties of each element of the mesh between steps, depending on the last step results, please let me know.

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Barcelona






+-------------------------------------------------------------+
| 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
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