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

You are not logged in.

#1 2009-09-16 09:02:04

bene
Member
Registered: 2009-03-06
Posts: 10

Large plastic deformations - Simo_Miehe for shells?

Hi forum, it's me again.

This time I have a question about an analysis including large plastic deformations.
I try to simulate a plastic tube, that has several folds in it. (I included a picture for your better understanding). One side of the tube is constrained, the other side is closed with a stiff cap.
Now I define an increasing inner pressure, in other words I inflate the tube.
What I wanna see is, that while the tube inflates and expands, the folds flatten more and more until the tube is almost plain, somewhere at this point the material model should fail and there should be divergence.
The point of failure should be somewhere between 4 and 5 bar in reality, ANSYS and Abaqus which I both used for validating my Code_Aster-results do tell me something like that.
But the strange thing is, that CA reaches almost 8 bar before diverging.
The obvious reason is, that my model behaves much to stiff in C_A, the folds do not flatten in the same manner they do in ANSYS/Abaqus. Hence I do get the biggest plastic strains at the wrong place in my model. So I varieed the element types, and now here we go with the story:

Originally, my model consists of linear quad4 shell elements. But if I understood right what I read in the documetation and this forum, these elements are supposed to be plain, so I can't use them.
Furthermore „Simo_Miehe“, what I wanted to use, is not implemented for them.

I then used linear hex8-elements with Simo-Miehe. That is the case I mentioned above: It converges, but behaves to stiff. Because of that, I wanted to use reduced integrated elements (3D_SI) because of their reduced stiffness, but then CA tells me, that Simo-Miehe is not implemented for them as well. 

Okay, lets try quadratic hex20. They seem to behave better, but still they don't represent the flattening of the folds and diverge way to late. Besides, the computational time is painfully long with them. I know, that the discretisation with quadratic elements may be much coarser, but my geometry demands a relatively fine meshing.

So right now, I changed to quadratic shells and modelisation type „coque_3D“. But the documentation and CA itself indicate me, that I then have to use deformation type „Green_GR“, which isn't correct in my eyes, since I do have large deformations.

So as a summary, my big question is:
Which combination of element type and deformation type is suited to represent my model behaviour?
I can't believe that there is no way to reach better results, I just think that I didn't get right everything by now!

Thanks in advance for your advices.
Attached you find an document with some pictures. If demanded, I can also post one of my inputs here, but since I don't get execution errors and my simulation obviously goes in the right direction, I thought it is not necessary.

Have a nice day -

BeNe


Attachments:
tube.pdf, Size: 1.28 MiB, Downloads: 652

Offline

#2 2009-09-16 10:07:42

Thomas DE SOZA
Guru
From: EDF
Registered: 2007-11-23
Posts: 3,066

Re: Large plastic deformations - Simo_Miehe for shells?

Hi there,

bene wrote:

So as a summary, my big question is:
Which combination of element type and deformation type is suited to represent my model behaviour?
I can't believe that there is no way to reach better results, I just think that I didn't get right everything by now!

This one is hard to answer, I'd rather try to answer all your questions the best I can (see below). Out of curiosity could you provide more insight of what model, hypothesis are used in Abaqus and Ansys for this computation ?


bene wrote:

Originally, my model consists of linear quad4 shell elements. But if I understood right what I read in the documetation and this forum, these elements are supposed to be plain, so I can't use them.
Furthermore „Simo_Miehe“, what I wanted to use, is not implemented for them.

DKT, DSG and Q4G as explained in U3.12.01 must use plane elements (that is for QUAD4 elements, all four nodes must be on a plane).
COQUE_3D is the only shell element in Code_Aster that takes into account the curvature of the geometry (with quadratic elements).
Moreover COQUE_3D supports non-linear geometry (large displacements, large rotations), but does not support large deformations.

bene wrote:

I then used linear hex8-elements with Simo-Miehe. That is the case I mentioned above: It converges, but behaves to stiff. Because of that, I wanted to use reduced integrated elements (3D_SI) because of their reduced stiffness, but then CA tells me, that Simo-Miehe is not implemented for them as well.

This is strange, are you sure about that ? Did you make sure that you applied both '3D' and '3D_SI' in AFFE_MODELE (this is important)
And did you make sure you used HEXA20 elements ?

bene wrote:

Okay, lets try quadratic hex20. They seem to behave better, but still they don't represent the flattening of the folds and diverge way to late. Besides, the computational time is painfully long with them. I know, that the discretisation with quadratic elements may be much coarser, but my geometry demands a relatively fine meshing.

You may try another alternative. Instead of using 3D or 3D_SI, try to use 3D_INCO_GD (which is dedicated to large plastic deformations). It also uses reduced integration as well as additional unknowns to enforce plastic incompressibility. As with 3D_SI you must use HEXA20 elements for that.

bene wrote:

So right now, I changed to quadratic shells and modelisation type „coque_3D“. But the documentation and CA itself indicate me, that I then have to use deformation type „Green_GR“, which isn't correct in my eyes, since I do have large deformations.

As said above, GREEN_GR enforces exact geometry but still implies a small deformation hypothesis.

TdS

Offline

#3 2009-09-17 08:18:22

bene
Member
Registered: 2009-03-06
Posts: 10

Re: Large plastic deformations - Simo_Miehe for shells?

Hi Thomas,

first of all, thank you for your detailed review of my problem!
I think I do it the same way as you did, and comment everything step by step.

Thomas DE SOZA wrote:

Hi there,

This one is hard to answer, I'd rather try to answer all your questions the best I can (see below). Out of curiosity could you provide more insight of what model, hypothesis are used in Abaqus and Ansys for this computation ?

To be honest, I can't tell you much about that right now, because I'm still a newbie to all these theories. As far as I know, almost all element types in ANSYS/Abaqus are able to take into account large deformations. Furthermore, if you use NLGEOM, large rotations and displacements are computed, if the chosen element type is suitable to do that.
I hope that my elements are, but I will have a look into it! In Ansys I used either fully integrated linear hex8-elements or linear hex8-elements with enhanced-strain modeling. In Abaqus I chose lin hex8 with incompatible modes, which is comparable to the enhanced-strain elements, as far as I know.

Thomas DE SOZA wrote:

DKT, DSG and Q4G as explained in U3.12.01 must use plane elements (that is for QUAD4 elements, all four nodes must be on a plane).
COQUE_3D is the only shell element in Code_Aster that takes into account the curvature of the geometry (with quadratic elements).
Moreover COQUE_3D supports non-linear geometry (large displacements, large rotations), but does not support large deformations.

Ok, didn't figure that out this detailed yet. Thanks for that!

Thomas DE SOZA wrote:

This is strange, are you sure about that ? Did you make sure that you applied both '3D' and '3D_SI' in AFFE_MODELE (this is important)
And did you make sure you used HEXA20 elements ?

Another thing I quite didn't know. I didn't use hex20 but hex8, that explains why it didn't work! Because up to now, I never had the need to use reduced integrated quadratic elements. For me, in most cases it makes sense to take reduced integrated linear elements, to weaken the stiffening effect of shear locking (which does not appear with quadratic elements).

But please tell me: Why do I have to apply both 3D and 3D_SI? How does the solver decide which formulation to use for which element? Or is 3D like a keyword to enable 3D_SI?

Thomas DE SOZA wrote:

You may try another alternative. Instead of using 3D or 3D_SI, try to use 3D_INCO_GD (which is dedicated to large plastic deformations). It also uses reduced integration as well as additional unknowns to enforce plastic incompressibility. As with 3D_SI you must use HEXA20 elements for that.

Thanks for that advice, I will have a look into the documentation because I would like to try that! Biggest problem right now is the computational time, the model is just too large with quadratic elements and I should have results by the end of the week.

Thomas DE SOZA wrote:

As said above, GREEN_GR enforces exact geometry but still implies a small deformation hypothesis.

Yeah, thats still my problem. I'll have to see what results come up from the calculation which is running right now (and uses 3D_SI thanks to your answers).

Once again, thank you for your professional help!

BeNe

Offline