Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2020-08-11 17:15:38

sonerc
Member
Registered: 2020-08-07
Posts: 9

Thermomechanical analysis using 3D SHELL elements - Possible?

Hi everyone,

Does CodeAster support the use of 3D shell elements for thermomechanical analyses? I would like to simulate the thermal expansion of a 3D, thin and wide part and I think the best way to model this problem is using 3D shell elements. I couldn't perform this in Salome Meca. I used the following for the initial thermal stage:

model = AFFE_MODELE(
  AFFE=_F(
    MODELISATION=('COQUE', ),
    PHENOMENE='THERMIQUE',
    TOUT='OUI'
  ),
  MAILLAGE=mesh
)

But I got an error saying that none of the nodes in the mesh has temperature DOF (Vous voulez contraindre le ddl TEMP sur un ensemble de noeuds, Mais ce ddl n'existe sur aucun de ces noeuds.).

Other modelisation options available are:
3D, AXIS, and PLAN but non of these are suitable for 3D shell type elements. Is that right?

I would appreciate any suggestion.

Thank you in advance

Offline

#2 2020-08-12 07:20:09

mf
Member
Registered: 2019-06-18
Posts: 93

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Hi,

I haven't tried this with COQUE elements, but U3.12.03 says:

The   application   of   a   thermal   loading   of   dilation   is   carried   out   by   defining   the   keyword   factor AFFE_VARC under AFFE_MATERIAU [U4.43.03].

So the application of a thermal load is done by AFFE_MATERIAU. Just like in the following post, but there with POU_DE:

h ttps://code-aster.org/forum2/viewtopic.php?id=24669

(delete the blank, no links allowed)

Typically, you do not do a separate thermal stage in such a calculation, you just assign temperatures. Due to nonlinear material (at least two temps) it must be STAT_NON_LINE.

Let us know if it worked,

Mario.

Last edited by mf (2020-08-12 07:31:18)

Offline

#3 2020-08-12 09:29:05

sonerc
Member
Registered: 2020-08-07
Posts: 9

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Hello Mario,


Thank you for your reply. I will try this and post back. It might take a bit of time as I am new to CodeAster. But skipping the thermal analysis stage sounds like an effective workaround as I will use a uniform temperature increase.

Thank very much,

Soner

Offline

#4 2020-08-12 10:38:43

sonerc
Member
Registered: 2020-08-07
Posts: 9

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

I have tried to follow your suggestion as closely as possible. As a result I ran into an error (below) that I do not really understand. I couldn't find information on the keyword "NSPG_NBVA" either. Any suggestions as to what I might be doing wrong? COMM and MESSAGE files are attached.

Thank for your help,
Soner

   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
   ! <S> Exception user raised but not interceptee.                !
   ! The bases are fermees.                                        !
   ! Type of the exception: error                                  !
   !                                                               !
   !  the computation of the option:  NSPG_NBVA                    !
   !  is not possible for any the types of elements of the LIGREL. !
   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
fine CR of execution of JDC in MIXTE

REPORT
>> JDC.py: FIN REPORT
EXECUTION_CODE_ASTER_EXIT_3119=0


Attachments:
COQUE3D_thermal.zip, Size: 9.82 KiB, Downloads: 17

Offline

#5 2020-08-12 11:27:41

mf
Member
Registered: 2019-06-18
Posts: 93

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Hi,

I don't know about this error but I miss AFFE_CARA_ELEM in your .comm. You did not define any thickness of the shells.

Take a look at example SSNV141 (search for it in your installation folder) and read the according documentation of AFFE_CARA_ELEM h ttps://www.code-aster.org/V2/doc/default/en/man_u/u4/u4.42.01.pdf

Mario.

Last edited by mf (2020-08-12 11:28:51)

Offline

#6 2020-08-12 16:13:25

sonerc
Member
Registered: 2020-08-07
Posts: 9

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Mario,

Thank you for your reply. Indeed I forgot to assign the shell thickness in the previous model. However when I include it I got some other errors (didn't expect otherwise big_smile).

In case someone would face the same issues:
-----------------------
The 1st error was:

"Aucune maille du maillage mesh n'a été affectée par des éléments finis. "

Solution: Following the suggestions in this post (https://w   ww.code-aster.org/forum2/viewtopic.php?id=23517) I converted my mesh to bi-quadratic type in Salome Meca.
------------------------
2nd error was:

"The computation of the option CHAR_MECA_TEMP_R is not possible. It misses the CARA_ELEM."

Solution: I forgot to add CARA_ELEM in STAT_NON_LINE.
--------------------------

Now I am stuck at a MatriceSinguliereError...

The mesh and model are pretty simple so I don't think it's a problem with boundary conditions etc. I attached the message and MED files. Any feedback would be much appreciated!

Soner


Attachments:
Result-Stage_1.zip, Size: 15.21 KiB, Downloads: 17

Offline

#7 2020-08-12 17:28:51

mf
Member
Registered: 2019-06-18
Posts: 93

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Hi,

your GROUP 'fix' also has DOFs in rotation. Your body is able to rotate around the X-axis ---> singularity.

Set all DRXi=0 in 'fix' and it should work.

Mario.

EDIT: My mistake, of course, DRX=0 is sufficient.

Last edited by mf (2020-08-12 17:41:24)

Offline

#8 2020-08-13 09:25:27

sonerc
Member
Registered: 2020-08-07
Posts: 9

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Mario,

Also my mistake, fixing DRX=0 solved the error and the simulation ran without warnings/errors. Thank you very much again! However the results look strange...

Please see the attached image (scale factor = 100). It seems like temperature difference is trying to displace the nodes but element centers seem to be fixed in space(hence creating spikes in the image). The maximum deformation seems reasonable (0.1 m of expansion of 100 m steel plate under 100C temperature change...).

Also I couldn't visualize stress or strain fields on the elements. I tried SIEQ_ELGA, SIGM_ELGA but they do not show up in ParaVis.

Any suggestions?

Soner


Attachments:
Untitled.png, Size: 342.39 KiB, Downloads: 25

Offline

#9 2020-08-13 10:49:11

mf
Member
Registered: 2019-06-18
Posts: 93

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

Hi,

unfortunately, I am not very experienced when it comes to shell elements. It seems that not all nodes are affected by your temperature assignment, or not all nodes follow the thermal expansion.

I am not sure if your choice of elements is correct or applicable. Try changing to 1st or 2nd order elements and see if it persists....

Mario.

EDIT: I do not know what CA does when COQUE_3D are used and your GEO has an angled surface like you have. It may be possible, that the COQUE elements are placed with the same angle as in the segment next to it. So basically, their base vector might not be correct in the angled segment....but, as I said, I'm not too experienced with elements COQUE...

Last edited by mf (2020-08-13 10:56:22)

Offline

#10 2020-08-14 07:30:26

sonerc
Member
Registered: 2020-08-07
Posts: 9

Re: Thermomechanical analysis using 3D SHELL elements - Possible?

I see, thanks for your help up to this point it was extremely useful smile

I will try to dig deeper in why the COQUE_3D element centers behave strangely in my model while the nodes seem to give correct results (I compared with 3D modelisation and values I get at nodes of the COQUE_3D elements are in agreement with 3D elements except for stress results which is surprisingly half of what I get with 3D elements).

I will post here if I can find anything. If anyone else have any suggestions please let me know.

Kind regards,
Soner

Offline