[SOLVED] Solids Elements with COQUE_3D Skin

toltec · 2012-08-21 17:27:29

Hello All,

I'm building a non-linear model (STAT_NON_LINE, VMIS_ISOT_TRAC, GROT_GDEP) which will undergo large rotations (car suspension). I cannot use LIAISON_SOLIDE to connect parts as these constraints should not be used with GROT_GDEP (they generate significant stresses). I have therefore used COQUE_3D elements as a skin over solid elements to act as connectors. The attached screen dump shows a "bolt" connection.

To cut a long story short, the model works well with the exception that the "skin" shells generate significant stresses if the unloaded mechanism is rotated. That is, when rotating the suspension (with all forces removed for testing) I would expect zero stresses in the "bolts", but 20MPa is typical. Have I missed something about Aster that makes this model set-up wrong?

Any ideas would be greatly appreciated!

Cheers

Gary

PS I've checked hinge alignment, so forces are not being generated by misalignment.

Last edited by toltec (2012-08-24 09:25:28)

Attachments:
Screenshot from 2012-08-21 17:13:23.png, Size: 254.69 KiB, Downloads: 333

Thomas DE SOZA · 2012-08-22 07:34:02

toltec wrote:

That is, when rotating the suspension (with all forces removed for testing)

How did you apply this rotation ?

TdS

toltec · 2012-08-22 12:29:18

Hi Thomas,

Attached is a document showing my set-up. Rotation occurs by defining a translational displacement at a node which causes the structure to rotate. Unexpected stresses develop at any shells that move.

As a matter of interest when applying a thin shell layer (0.1mm) on the green part these shells also generate stresses in some areas as the structure rotates. Perhaps this has something to do with the shell normals? I've arbitrarily defined them as ANGL_REP=(0,1,)

Cheers

Gary

Attachments:
shell-skin.ppt, Size: 533.5 KiB, Downloads: 440

Thomas DE SOZA · 2012-08-22 17:21:01

Hi,

That's an interesting model but I don't really understand how the connection between the shells and 3D work.

Where's there's stress, there strain, maybe you should try to plot the deformation (EPSI_XXXX) on the whole structure to find if there's a particular spot in the shells where the deformation is very high and could explain the high stresses.
This may give some clues.

TdS

toltec · 2012-08-23 09:54:53

Greetings Thomas,

The shells are intended to stand in for LIAISON_SOLIDE elements in a GROT_GDEP analyses, so they line the holes in the 3D elements and also close the holes. Loads/BCs will be applied to these shells and other parts will connect to them.

To clarify this, attached is a simplified model which demonstrates how these shells generate stresses even though forces in the structure are minimal. I've also included a document describing this model.

Many thanks for to you for your help and for anyone who cares to jump in.

Cheers

Gary

Attachments:
edf_example.comm.tar.gz, Size: 714.03 KiB, Downloads: 334

Paul CARRICO · 2012-08-23 12:31:24

Hi,

Why don't you use 3D elements instead of shell elements (even if you want to post-process the efforts of the screws) ?

Furthermore, It mmay be better to impose the displacement on the (group) faces of the part rather than on a single node, otherwise you'll have troubles ...

only few parts with structured elements ... :-))

As Thomas said, interesting (nl) modelling

Paul

toltec · 2012-08-23 13:40:15

Hi Paul,

Thanks for your post. Using solids for connectors is a good idea... probably a better strategy given that that is how real world connectors work!

I am however still uncomfortable as to why unloaded shell elements on the face of rotating,unloaded solids produce stress. Either I don't understand something, or the COQUE_3D formulation has a problem with this technique.

Gary

Thomas DE SOZA · 2012-08-23 15:25:06

toltec wrote:

I am however still uncomfortable as to why unloaded shell elements on the face of rotating,unloaded solids produce stress. Either I don't understand something, or the COQUE_3D formulation has a problem with this technique.

Looking at your command file, I think it may come from the dummy torque stiffness that every shell carries about its normal. It is setup using the keyword COEF_RIGI_DRZ in AFFE_CARA_ELEM and must be non zero.
Without this stiffness you would have been unable to apply the push load. This stiffness implies that the shells will deform and may therefore generate stresses. Moreover the sharp edges in the bolts will allow this stress to be transferred to the solid (this is what can be observed on the SIEF_ELGA field).

I'm afraid there is no easy workaround to this matter.

TdS

Paul CARRICO · 2012-08-23 15:35:41

Why don't you basically stick the 2 parts, considering the tightening cone of 45 degrees ?

toltec · 2012-08-23 16:47:37

Thomas, Paul,

Thanks for your suggestions and input. The shell stresses do indeed decrease if I lower the drill stiffness, so at least I now understand what's going on. It's interesting though that a model consisting only of COQUE_3D elements doesn't produce these stresses when rotated. Although these shells are all in the same plane...

Thanks again.

Gary

Last edited by toltec (2012-08-23 17:07:41)

#1 2012-08-21 17:27:29

[SOLVED] Solids Elements with COQUE_3D Skin

#2 2012-08-22 07:34:02

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#3 2012-08-22 12:29:18

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#4 2012-08-22 17:21:01

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#5 2012-08-23 09:54:53

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#6 2012-08-23 12:31:24

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#7 2012-08-23 13:40:15

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#8 2012-08-23 15:25:06

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#9 2012-08-23 15:35:41

Re: [SOLVED] Solids Elements with COQUE_3D Skin

#10 2012-08-23 16:47:37

Re: [SOLVED] Solids Elements with COQUE_3D Skin

Board footer