Contact with SIMO_MIEHE

rupole1185 · 2022-01-25 10:26:02

Hi there,

I have a problem to be handled (for which I can't share the mesh as it's under SLA with a client, but I try my best to make you understand it). The situation I am simulating consists of a gasket which is squeezed in between a housing and a cover. The gasket is made of steel which, due to the squeezing, goes into plasticity zone.

Everything is made of extruded prisms (so 3D modelling). To simulate this I made obviously a contact as follows:

contact = DEFI_CONTACT( FORMULATION='CONTINUE', RESI_GEOM=0.01, MODELE=model,
ZONE=_F( GROUP_MA_ESCL=( contact_slave_surface, ), GROUP_MA_MAIT=( contact_master_surface, ),), )

I made several attempts using STAT_NON_LINE but they all failed. For STAT_NON_LINE I use this configuration:

stat2 = STAT_NON_LINE(
CARA_ELEM=elemprop,
CHAM_MATER=fieldmat,
CONTACT=contact,
EXCIT=loadr,
COMPORTEMENT=comportement,
INCREMENT=_F(LIST_INST=times, INST_FIN=listr.Valeurs()[1], ),
NEWTON=_F( MATRICE='TANGENTE', PREDICTION='TANGENTE', REAC_INCR=1, REAC_ITER=1, ),
ARCHIVAGE=_F(PAS_ARCH=SaveFreq),
CONVERGENCE=_F(ITER_GLOB_MAXI=80, RESI_GLOB_RELA=1e-4,),
MODELE=model
)

where comportement is:

comportement=(_F(TOUT='OUI',
RELATION='ELAS',
DEFORMATION='PETIT',
RESI_CPLAN_RELA=1.E-06,
RESI_INTE_RELA=1.E-06,
ITER_INTE_MAXI=20,
ITER_INTE_PAS=0,
ITER_CPLAN_MAXI=1,
SYME_MATR_TANG='OUI',
PARM_THETA=1.0,),
_F(GROUP_MA=('LAY_3D_1', ),
RELATION='VMIS_ISOT_LINE',
DEFORMATION='SIMO_MIEHE',
RESI_CPLAN_RELA=1.E-06,
RESI_INTE_RELA=1.E-06,
ITER_INTE_MAXI=20,
ITER_CPLAN_MAXI=1,
SYME_MATR_TANG='OUI',
PARM_THETA=1.0,),)

But all the attempts I made using STAT_NON_LINE fail with an Error like this:

__________________________
<Erreur> Échec dans l'intégration de la loi de comportement

<Action> On essaie de découper le pas de temps.
On utilise la découpe manuelle.
Découpe uniforme à partir de l'instant < 0.000000000000e+00> en <2> pas de temps.
(soit un incrément constant de < 8.333333333333e-03>)
Le nombre maximal <2> de niveaux de subdivision est atteint.
<Action><Échec> Échec dans la tentative de découper le pas de temps.
__________________________

I tried then to use DYNA_NON_LINE with a similar configuration and the process gets a bit better but I am forced to use an incredibly small time step (i.e. 1E-3) which means I may get results in a very long time or, if I am less lucky, the simulation gets stuck after several hours with the same error mentioned before.

I know that without mesh it's difficulto to help, but if someone have had experiences about this maybe he can try and share them!

piotr.kozlowski · 2022-01-26 14:17:44

Hi rupole1185,

it could be couple of things, as you probably know.
1. I would try to change the material to linear elastic formulation and check if the analysis converges.
2. I would also try to ramp the "squeezing" at a lower rate.
3. How many elements does the gasket have through thickness? Can you make a snapshot showing the contact region of the gasket/housings? Try changing the contact do bonded ad see if it converges.

By checking 1,2, and finally three you might get a better idea about where the problem is.

Regards,
Piotr

rupole1185 · 2022-01-26 16:48:27

Hi piotr,

thanks for your reply. About your points here you are my answers:

1. I would try to change the material to linear elastic formulation and check if the analysis converges.

-> yeah, I confirm that linear analysis converges towards a result. The experimental data are not coherent with that and for this I need to turn on plasticity

2. I would also try to ramp the "squeezing" at a lower rate.

-> On this term I think I tried everything. I tried lowering this rate both by adding time steps and reducing the FONC_MULT

3. How many elements does the gasket have through thickness? Can you make a snapshot showing the contact region of the gasket/housings? Try changing the contact do bonded ad see if it converges.

-> in the most recent I placed 3 layers of extruded tetrahedron as in the attached picture. I can add some more, but the computational time increases a lot (it's several hundred thousands cells). About maing the contact bounded it is not possible as at the beginning the gasket surface is not flat, it becomes flat after the pressure from the housing and the cover.

Attachments:
thikness.jpg, Size: 182.04 KiB, Downloads: 145

piotr.kozlowski · 2022-01-26 17:23:38

Is it a displacement or force-controlled problem?
I don't have experience with the elements you are using there for the gasket, but if the elastic model converges then I would look closer at the material properties. In particular the definition of the tangent modulus. Have you tried to increase the tangent modulus for the elastoplastic material?

rupole1185 · 2022-01-26 17:35:22

piotr.kozlowski wrote:

Is it a displacement or force-controlled problem?
I don't have experience with the elements you are using there for the gasket, but if the elastic model converges then I would look closer at the material properties. In particular the definition of the tangent modulus. Have you tried to increase the tangent modulus for the elastoplastic material?

It's a force controlled problem. I tried that as well, but so far I have had poor results also using this [or better, the simulation is still running but it is very long and so I can't tell you if this can be a solution ...].

Are there other modelling possibilities you could reccomend? I didn't use shell as I am not sure whether shells can be compressed in between two surfaces. Do you know if this is possible?

piotr.kozlowski · 2022-01-26 19:56:47

It depends a bit on the results you are after but in general, you could use the shell elements to represent a stiffness of a waved gasket. But I cannot give you a lot of advice on what modelization to use. I have some experience with metal forming simulations and usage of shells, but not in Code Aster.
Perhaps you could try building a simpler mesh: two solid blocks with a waved strip of "gasket" in-between to check various modelizations.

Do you use an automatic time step decrease method if non-convergence occurs: DEFI_LIST_INST, METHODE=AUTO?
Can you share your mess file?

rupole1185 · 2022-01-26 20:48:34

Attached you find a mesh and a message.dat file in a very much simplified situation with a small drawing representative of the situation.

I start being a bit desperate about this case as I worked on it for 10 days in order to make it converge and still I didn't manage.

rupole1185 · 2022-01-26 20:52:50

And the attachment I forgot in previous post

Attachments:
schema.zip, Size: 206.32 KiB, Downloads: 151

AsterO'dactyle · 2022-01-26 22:04:05

Hello,

With contact, PREDICTION='ELASTIQUE" is a good idea

rupole1185 · 2022-01-26 22:09:07

AsterO'dactyle wrote:

Hello,
With contact, PREDICTION='ELASTIQUE" is a good idea

Hi, thanks for the hint. I tried that but with no luck...

konyaro · 2022-01-27 10:43:17

Hello,
I often come across that problem. Contact analysis + GDEF_LOG or SIMO_MIEHE often leads to that error even if the parts shouldn’t meet large deformation. I saw the new option CONT_STAT_ELAS recently but couldn’t try yet as I’m still working with an old version. What I can nevertheless advise you:
- Check the quality of your mesh and try to improve it if needed, for instance by increasing the number of optimization steps in Salome.
- Add some discrete elements to all nodes of your spring in order to increase the stiffness of your model. That changes the results of course but sometimes a compromise can be found in order to reach convergence with satisfying results.

Good luck,
Konyaro

Last edited by konyaro (2022-01-27 10:45:26)

piotr.kozlowski · 2022-01-27 11:26:14

Hi rupole1185,
How did the analysis with increased tangent modulus go?
I have not looked at the files you sent yet.

The fact your analysis converges with fully elastic material is good news I think. I would explore the material properties and make it a displacement control problem with small enforced displacement. If you will have some results to look at then maybe you could eyeball potential issues with the mesh being deformed etc.

rupole1185 · 2022-01-29 17:42:25

Hi there,

thanks a lot for the multiple replies first of all. I keep investigating on this issue which I have not completely solved. Currently I am working on the simplified model I put here and I managed to make it converge. I had to modify the whole model substantially. In particular:

1) I had to add several springs (DIS_TR). They stabilise a lot the simulation and, even if they affect the results a little bit, I noticed you can't make it without them

2) I had also to work on the mesh. I very much refined the mesh (keeping under control the quality)

With this two updates I managed to make the SIMO_MIEHE material converge (with a little time step). In the coming week I try the same solution on the big model I have and I really hope this works.

In any case, we are talink of VERY slow simulations: on my mesh which are something like 1.000.000 nodes it could take more than 24/48 hours to get the results ... and this is not very good either.

#1 2022-01-25 10:26:02

Contact with SIMO_MIEHE

#2 2022-01-26 14:17:44

Re: Contact with SIMO_MIEHE

#3 2022-01-26 16:48:27

Re: Contact with SIMO_MIEHE

#4 2022-01-26 17:23:38

Re: Contact with SIMO_MIEHE

#5 2022-01-26 17:35:22

Re: Contact with SIMO_MIEHE

#6 2022-01-26 19:56:47

Re: Contact with SIMO_MIEHE

#7 2022-01-26 20:48:34

Re: Contact with SIMO_MIEHE

#8 2022-01-26 20:52:50

Re: Contact with SIMO_MIEHE

#9 2022-01-26 22:04:05

Re: Contact with SIMO_MIEHE

#10 2022-01-26 22:09:07

Re: Contact with SIMO_MIEHE

#11 2022-01-27 10:43:17

Re: Contact with SIMO_MIEHE

#12 2022-01-27 11:26:14

Re: Contact with SIMO_MIEHE

#13 2022-01-29 17:42:25

Re: Contact with SIMO_MIEHE

Board footer