convergence problem with symmetry boundary conditions

vishwas

Hi,
I am trying a crimping simulation as bshown below.

It has has symmetry bcs on two quarter planes as shown below in schematics.

the problem is I am getting singular matrix error. For friction II tried all variants including:
turning on SANS_GROUP_NO for t_exclude group
turning on SANS_GROUP_NO_FR
disabling friction entirely
ALSO FOR TOOL MOTION I GET SINGULAR MATRIX IF IMPOSED MOTION IS THRU AFFE_CHAR_MECA,WHY SO
Changing from AFFE_CHAR_MECA to AFFE_CHAR_CINE for tool motion also doesn't get help converge till end.
The inner tube is applied hyperelastic material and has significant problems in convergence(its a metal-rubber contact problem) The VARI_CONT number never goes to zero in terminal column.
All groups are created including trimmed groups that eliiminate shared edges(or nodes) between contacting faces and symmetry faces.
Please find attached study here:https://www.dropbox.com/scl/fi/uejz17m2gogji4t8ek77m/crimp.tar.xz?rlkey=0yxjhhrrkdv8cr4qitiwo669u&st=n3d1jjlj&dl=0

I was able to get good results without much fuss using Calculix Solver. Please see here https ://youtu.be/2qUt8ZQsU-M

Thanks and Regards
Anirudh Nehra

vishwas

Hi,
I tried a run mentioned here with friction https://forum.code-aster.org/public/d/19959-solved-no-convergence-if-friction-is-activated
and it ran without issue in latest 17.4.0 release.

Regards
Anirudh

vishwas

Hello,
Any inputs are greatly appreciated.

Regards

Sound_Spinning

vishwas
Hi, I had a 1st (very quick) glance at your input deck & mesh. Before I duplicate stuff you may have tried, I have a couple of questions:

the tools show an initial gap of about 0.7mm. Is it not better with NL contacts to start with those moved on top of the contact surfs? When I run your deck it only solves about 0.5mm of the gap; i.e. no contact started.
if you make the tools as 'masters' for the contact, don't you need a finer mesh on the tube (slave) side for them to make more sense?
Have you tried high-order meshes with mid-nodes projected onto the cyl geometry? So you get the curvatura right at the start of the contact?
When you did this in CCX, did you use exactly the same low-order mesh, and did it solve OK?

Sound_Spinning

vishwas
Also, when I try to run your model, I get this in the message file after applying element types to the mesh:

Those 4240 elems seem to tie up with the number of solid_shells you created? Have you found out what the warning above is about?

Have you tried to solve the model with 'normal' bricks, before you create the solid_shell ones?

Sound_Spinning

Hi, here is a model which does 'something' in 6 load increments. I removed the friction & the solid_shell bricks (see warning posted above, maybe find out more about them?). There were quite a number of things needed to be improved, including over-constraints and I removed all non-default entries to do with NL solvers. Made them all more generic and let the solver to do its job. I made the period = 3, so that time steps match your displacement load on tools in mm.

Here is a .zip with input & results files: crimping.zip
See hand edits in .COMM file, search for JB edit.

Maybe pull the string from this model wrt friction & see if you get the solid_shells to work. If you do, I'll have a look how to plot the assy with those in PV.
Out of curiosity, what do solid_shells bring to the plate that usual solids don't? Have never used them.

vishwas

Hi,
Thanks for responding.
1> initial gap should not make much difference. There Is always a gap in real assembly. The software should handle those easily. Infact if you disable contact altogether it will converge easily.
2> you are confusing master slave assignment.
crimp_sl is master and tool faces slave. crimp_sl cannot be slave to tool faces because then same slave in more than 1 contact zone which leads to fatal error.More info in "Note on use of contact."
3>I have created every possible group of nodes(nodes on sym faces etc for redundant DOF eliminating) and tried every possible combination under contact settings. When not working, included LIAISON_MAIL to mimic "bonding contact" behavior but still has problems.
4> If you deactivate both contact and LIAISON_MAIL between tube and crimp body, it converges easily and s solves contact between tools and crimp body.
Solid shell will revert back to 3D if Assignment fails in AFFE_MODELE. But they seem to be assigned because they need GDEF_LOG. They need HEX elements only and so more work meshing. I wanted PENTA to work but doesn't work unfortunately.
It looks like you removed symmetry and fix on inner tube(so it flexes more)
I'll have a look soon.
Too tired to work on this model.
Regarding Solid Shell elements see here: https://www.google.com/url?sa=t&source=web&rct=j&opi=89978449&url=https://hal.science/hal-02483993/document&ved=2ahUKEwjDn6zZ-5-SAxXhSGcHHdkQNAsQFnoECB4QAQ&usg=AOvVaw2RnwDZr8oST7Fa4NeakunG
They have many advantages over regular 3d brick or hex elements as seen in this research work.
As can be seen in link https://youtu.be/2qUt8ZQsU-M?si=EKZza3ESG4drUte7 , it works well in loading in calculix.(symmetry and elasto plastic and hyperelastic and contact-friction all work together which is the real goal of this simulation) with linear elements only.
you can see sticky behavior between tube and crimp
Regards

Sound_Spinning

vishwas
Have a look when not tired then. I reused your model sets, same. Removed loads of stuff. Your constraints were incorrect, you modelled a rigid cantilever with the shape of a 1/4 of a tube. The sym constraints were not honoured.
Have a look at my comments/notes in input file (.comm). I went past my initial posts as I realised about constraints. One thing at a time...

vishwas

Hi,
Thanks for reply. I am going through your comments. They are very informative.
I am running your model and one thing I noticed that I cannot change time step.
Neither more or less.
I changed from 0.17Xendtime to 0.1Xendtime and it failed(so as to have more timesteps at end since geom seems too distorted). Same if I changed to 0.2Xendtime.
I'll do more runs to check.
I don't understand what symmetry problems you tell. In an actual crimp machine, the crimp is held fixed and tools move in to press. I put in same constraints in calculix and it solved fine.
In this model I fixed inner tube face and it was successful. But the concerning fact is VMIS stresses are too high. With simple VMIS_ECRO_LINE (200 MPa Sy)

Regards
Anirudh

vishwas

Hello,
Result from calculix
You can see:
1>Symmetry boundary condition applied all over the front faces.
2>contact between tools and crimp. There is some interpenetration going on but thats due to sharp corner of tool.
3>frictional contact between inner tube(mooney-rivlin) tube and crimp body(elasto plastic steel)
4> The max vonmises stresses respect Stress strain hardening curve(elasto plasticity)
5>True sticky frictional response of tube with crimp due to pressure of tools. The tube squishes out due to load.
6>Robust contact detection between tube and crimp( contact opening/closing at one end)
6>fully fixed internal face of tube and crimp body(fix_1 and fix_cr groups in mesh)

Regards
Anirudh

Sound_Spinning

vishwas
Hi, your questions are fair, and I'd also like to know more on how the NL solvers work in CA, I'm quite new to them.

are you able to share the *.inp, input file, used in the CCX run, so I can have a look at it?
I also tried a smaller 1st load increment (<17% of 3mm) and fails, which it shouldn't; I agree.
If you need specific results at some time steps, better use the ARCHIVAGE entry inside the solve step; so we leave generic time stepping algo (auto_times in my deck) to do its job?
It is quite hard to compare 2 FEA solvers when you have several NL terms... e.g. I'd be very surprised if CCX (or any other FEA solver) got the stiffness right using low-order solids, they tend to be over-stiff.

Your stress- (plastic) strain curve in mat A7 looks like in graph below, was that the same in CCX?

Your entries on the linear hardening approach seem to have very high numbers?

SY (yield) = 205,000,000e6 Pa [?] & the slope very high?

vishwas

Yes, the stress strain curve in mat A7 is same as in calculix file.
MAT_1 is the one I copied from Simscale. I tried this model on Simscale platform(which use code_aster backend) but it failed on simscale as well.
MAT_1 I think is to make use GREEN_LAGRANGE deformation with elastic behaviour. GREEN_LAGRANGE signifies large displacements which cannot be used with ELAS by default. So, the trick is to use it with VMIS_ISOT_LINE with very large Yield Strength(which will never be reached during simulation) Here also D_SIGM_EPSI almost equal to E so, it has same slope even after SY.
When I said stresses are too high because I assigned ECRO_LINE(plast) material model to crimp with Yield Strength SY modified to 200 Mpa(and D_SIGM_EPSI like 2e4), So, it is bilnear hardening. But resulting VMIS stress are of order of 1E10 or more. It is not expected as with low Sy, it should soften up.(Calculix has peak stressesof 3e8Pa)

Anirudh

Sound_Spinning

vishwas
Thanks, I'll have a look when I get a minute.
A side note on Simscale: they recently switched the NL solver to Marc (Hexagon)? There may be a reason for it.
Keep you posted, I see better now what you were trying to do.

vishwas

Hello,
I don't think you will give it a shot but Here is the calculix .inp file - https://www.dropbox.com/scl/fi/bm7vg01k8ubz4i9gko8tj/allinone.inp?rlkey=ddmd7zoo2kqx2tka3r1ikyiaf&st=cmzjeghm&dl=0
The calculix model also has problem if I try to perform unloading operation. It fails at first time step during unloading(ie the tools retracting).
1-Yes, the stress strain curve in mat A7 is same as in calculix file.
2-MAT_1 is the one I copied from Simscale. I tried this model on Simscale platform(which use code_aster backend) but it failed on simscale as well.
3-MAT_1 I think is to make use GREEN_LAGRANGE deformation with elastic behaviour. GREEN_LAGRANGE signifies large displacements which cannot be used with ELAS by default. So, the trick is to use it with VMIS_ISOT_LINE with very large Yield Strength(which will never be reached during simulation) Here also D_SIGM_EPSI almost equal to E so, it has same slope even after SY.
4-When I said stresses are too high because I assigned ECRO_LINE(plast) material model to crimp with Yield Strength SY modified to 200 Mpa(and D_SIGM_EPSI like 2e4), So, it is bilnear hardening. But resulting VMIS stress are of order of 1E10 or more. It is not expected as with low Sy, it should soften up.(Calculix has peak stressesof 3e8Pa)
5- IMore disturbing fact is that If I turn on ALGO_CONT = 'PENALISATION' between tube and crimp, without friction, The contact is not even detected by solver. The crimp moves past tube body as seen below:

6- I am also trying a testcase SSNV506, which is a similiar model. It has symmetry on two planes and imposed motion.
When I activate friction It fails.

8-There is always LAGR dof causing singular matrix error in this testcase. Same in my model, LAGR_F2 between tool and crimp body cause singular matrix(even after using SANs_GROUP_NO_FR for removal of symmetry plane nodes, on some other node between crimp and tube)
Anirudh

Sound_Spinning

vishwas
I had a quick look at your *.inp, CCX deck:

you are solving the static step up to a period = 1.0; but your unloading part is after that?
your graph1 'drives' the loads (your disps on tools) as a ramp up to T=1, then unloading (amp=0) is between periods 1 and 2?
you may need to extend the period in a single step to 2; OR (recommended, at least from my Abaqus times) to add a Step#2 for unloading from 1 --> 2.
also, when using high friction (> 0.2) in Abaqus, and I think it is the same in CCX; you need to invoke the UNSYM solver, so that the full [K] matrix is solved?

PS: I am not sure CCX has an UNSYM parameter or not, but you should be able to see what solver is being used from the .log file in your CCX run? See like in this .log posted in the PrePoMax forum.
You'll see s'thing like this: Factoring the system of equations using the unsymmetric pardiso solver number of threads = 1

Sound_Spinning

vishwas
I had a quick flick thru the SSNV506 test help docs. It's full of caveats in the summary.... not sure about this NL solver and contacts as a general method, hard to crack / use it seems.

Sound_Spinning

I've checked that test above with solids, and they had an equation to hard link in Y the contact nodes on sphere & base.... Isn't that a cheat? They force those contact nodes to be together right from the start? Not a true contact?
LIAISON_DDL=_F(GROUP_NO=("S", "E"), DDL=("DY", "DY"), COEF_MULT=(1.0, -1.0), COEF_IMPO=0.0),

Very odd.....

vishwas

Hi,
I wouldn't call that cheat. Maybe for symmetry it wants to make sure both nodes move down together. Anyway it's a lot of work selecting those nodes. It becomes tiring to think of nodes on symmetry planes and conflicting with other BCs and then create groups over them and then eliminate using SANS_GROUP_NO etc. Or LIASION commands.
Maybe the issues I highlighted above could be addressed by some experts like-
1>I could partially make it work with only contact somehow but friction absolutely causes singular matrix.
2>even after solving contact without friction, results don't seem to be smooth and intuitive like calculix.(on crimp stress distribution)
3> The recommendation on removing lagrange DOFSs by using SANS_GROUP_NO and SANS_GROUP_NO_FR don't seem to be working.
4>Huge interpenetration when ALGO_CONT ='PENALISATION' is chosen for tube and crimp. As if there were no contact.

5>Even after turning off symmetry under EXCITE and eliminating every possible node which could come in conflict with BC, the run diverges in case of friction. Now some random node on tube - crimp interface show LAGS_F2 DOF singularity matrix error. This is the case even after turning off MUMPS singularity detection with NPREC = -1. Which makes hopes of converging very little already.
This after the mesh is all hex with perfectly aligned nodes lying on top of each other.

6>Last ditch effort to solve tube crimp contact -
to use LIAISON_MAIL and turn off contact altogether and even symmetry BCs
but in this case also the solver doesn't go past 30% of time.
7>Unable to mix contact zones of LAC and CONTINUE together.
8>All these things calculix also handled but without too much complaining.

Regards
Anirudh

mf

vishwas
Hello,

I don't want to hurt your feelings about Calculix, but your result has a lot of penetration. I mean: A LOT. So it is very likely far from correct at the edges of the tools (the first animation). And regarding CA/SM: if you do not respect the rules for contact (master mesh coarser than slave) what do you expect? I do not even expect it to run properly, so there is no sense in even arguing about the results. In the shared mesh, the meshes of the 3 tools are even different (!) in the contact zone.

Mario.

Sound_Spinning

vishwas
I've now read through this in help docs: Instructions for using contact in code_aster
It's full of many, many caveats, application dependant and/or loads of manual trial/error loops required for difficult (real?) cases.
See the parts about meshing, and even how with high-order elems more work is required for contacts... I don't think you can chuck just any mesh at it and hope for the best, loads of testing required to como up with a planned mesh for each case.

Nevertheless, I gave the test SSNV506 a shot:

I removed that equation in Y, makes no sense for such a simple model. It still solves, as expected. The model is driven by disps (constrained in Y) + sym planes and base constraints is enough. I called a 'cheat' (in a friendly manner, analyst's speak) coz it doesn't make for a general method. In real complex NL assys we shouldn't need those hacks on contacts.
Without friction + NL mats (yield = 50MPa), it seems to work fine, see signed von Mises, honoring the yield around 50MPa at base solid.

The help docs linked above recommends for friction to use the 'continue' solve method (I think?). As soon as I added friction, it doesn't solve. The num singularities I see imply that more manual work is required in the surf pairs, etc. I gave up, too much 'hacking' for such a simple example.

I think I'll just stick to all things linear in CA. I also found the NL dynamics solver with large rots, not playing ball at all w/out loads of hacking at strange modelling tricks even for a simple pendulum (see thread here).

What are your thoughts so far on all things NL in CA as a general method for 'real' assemblies?