Optistruct Plane Strain Error

Hi. I am preparing a simple 2D plane strain contact problem is Hypermesh for Optistruct. As you can see in the figure, the dark yellow bar is bonded two the blue, green and light yellow components and is fixed. The red bar applied with -Y displacement and it has frictional contact with the blue, green and light yellow components. For plane strain in PSHELL MID2=-1 is used, the CTPSTN and CQPSTN elements are used for tria3 and quad4 elements and also have assigned theta = 0 for CTPSTN and CQPSTN elements. But I am getting the following error for every elements. Please help me with it. I am also adding my model herewith.

This line was interpreted as:
7795:CTPSTN, 1002748, 12, 7312, 7298, 7326, 0.0

*** ERROR # 1000 *** in the input data:
Incorrect data in field # 7. Field 'G4' of CTPSTN bulk data.
Expected INT >= 0 or blank, found REAL (0).

Regards,

Debarshi

11.PNG

2D_Plane_Strain_Tesla_8_Seal_1_EPDM_E6MPa_02_02_2021.hm

plane_strain_element.PNG

PSHELL.PNG

Find more posts tagged with

Academic

English

Accepted answers

All comments

Adriano Koga_20259

Looks like it is not correctly supported by HyperMesh yet. It needs to be implemented by the development team.

It is exporting it wrong. I've tried it here in the newer version 2021 and got the same.

Nevertheless, your model needs to be at the base plabe XY or ZY, with base 0.0, and your model is not in accordance. Also the property for the Plane elements needs to use PPLANE. (newer implementation prefered over old PSHELL MID2).

I've changed a few things in your model, in order to make it work.

- Translated the model to XY plane, with base coord 0.0.

- changed all elements to 2nd order, and changed element types of all TRIA6 and QUAD8 to CT/CQPSTN, in order to be supported by HM export.

- assigned all elements with property PPLANE for planestrain

- changed contacts to N2S (node2surface), CONSLI (continuous sliding).

- changed loadstep to use NLPARM(LGDISP) for activating Large Displacement Analysis

- corrected SPCDs and SPC (applied just SPCD -1.0Y, and SPC 0.0 123456 in the top part)

Another workaround is to work with regular CTRIA/CQUAD elements, and after exporting, mannually change the element type to CTPSTN/CQPSTN, and watch for element node order. But this needs to be done in a text editor, and if you bring it back to HM, this will be lost.

2D_Plane_Strain_Tesla_8_Seal_1_EPDM_E6MPa_02_02_2021_rexport_2nd.zip

Debarshi

Looks like it is not correctly supported by HyperMesh yet. It needs to be implemented by the development team.

It is exporting it wrong. I've tried it here in the newer version 2021 and got the same.

Nevertheless, your model needs to be at the base plabe XY or ZY, with base 0.0, and your model is not in accordance. Also the property for the Plane elements needs to use PPLANE. (newer implementation prefered over old PSHELL MID2).

I've changed a few things in your model, in order to make it work.

- Translated the model to XY plane, with base coord 0.0.

- changed all elements to 2nd order, and changed element types of all TRIA6 and QUAD8 to CT/CQPSTN, in order to be supported by HM export.

- assigned all elements with property PPLANE for planestrain

- changed contacts to N2S (node2surface), CONSLI (continuous sliding).

- changed loadstep to use NLPARM(LGDISP) for activating Large Displacement Analysis

- corrected SPCDs and SPC (applied just SPCD -1.0Y, and SPC 0.0 123456 in the top part)

Another workaround is to work with regular CTRIA/CQUAD elements, and after exporting, mannually change the element type to CTPSTN/CQPSTN, and watch for element node order. But this needs to be done in a text editor, and if you bring it back to HM, this will be lost.

Hi Adriano,

Thanks for the quick response. It works. But I have few questions -

Is CT/CQPSTN only applicable for 2nd order elements?

Actually I have tried once by my own. I have changed your 2nd order elements to 1st order and then assigned CT/CQPSTN to respective elements again but got the same error as before.

'Another workaround is to work with regular CTRIA/CQUAD elements, and after exporting, mannually change the element type to CTPSTN/CQPSTN, and watch for element node order. But this needs to be done in a text editor, and if you bring it back to HM, this will be lost.'

Could you may be explain this a bit? I guess I am making some stupid mistake here.

Thanks and regards,

Debarshi

Adriano Koga_20259

Hi Adriano,

Thanks for the quick response. It works. But I have few questions -

Is CT/CQPSTN only applicable for 2nd order elements?

Actually I have tried once by my own. I have changed your 2nd order elements to 1st order and then assigned CT/CQPSTN to respective elements again but got the same error as before.

'Another workaround is to work with regular CTRIA/CQUAD elements, and after exporting, mannually change the element type to CTPSTN/CQPSTN, and watch for element node order. But this needs to be done in a text editor, and if you bring it back to HM, this will be lost.'

Could you may be explain this a bit? I guess I am making some stupid mistake here.

Thanks and regards,

Debarshi

The solver OptiStruct supports both 1st and 2nd order.

It looks like HyperMesh has an issue when exporting 1st order, and then the solver doesn't recognized it right.

Forget about the workaround. I thought the format of CQ/CQPSTN was similar to CTRIA/CQUAD, but it is not. you would need to use some good text esditor and record a script to change the first line to be the same as the second line here:

HM is not writting this as it should for 1st order.

Debarshi

The solver OptiStruct supports both 1st and 2nd order.

It looks like HyperMesh has an issue when exporting 1st order, and then the solver doesn't recognized it right.

Forget about the workaround. I thought the format of CQ/CQPSTN was similar to CTRIA/CQUAD, but it is not. you would need to use some good text esditor and record a script to change the first line to be the same as the second line here:

HM is not writting this as it should for 1st order.

Hi Adriano,

Thanks for the info. I have prepared the model as you have explained for the above mentioned boundary conditions. But now I am getting a different error. Could you may be help for it?

*** INTERNAL PROGRAMMING ERROR ***
in file "csl2de2_kfnl.F", at location # 530.

**** ABORTING RUN DUE TO AN INTERNAL ERROR ****

************************************************************************
OptiStruct error termination report printed to file
"test.stat".
Additional information may be found from standard streams stderr/stdout.
These are usually directed to the terminal, or collected
as separate files by any queuing or remote execution systems.
HyperWorks RunManager shows stderr in a separate 'log' window.

I got this error after 40% load step have been completed.

I am attaching the files.

Thanks and regards,

Debarshi

test.fem

test.hm