I wish to do it but for that I need to produce a deformation mode and/or stress results that shows that component will fail
The current simplified compression test is throwing convergence issues, but I can try with your idea to see if it works
I agree completly, I have also kept friction coefficent at 0.3. I noticed that with or without friction coefficent the convergence issues remained same. Still I will drop the friction coefficient from now on
Because they seem to be related more to mesh distortion/large deformation. There was a similar case with suspected friction issues though: Hyperelastic contacts in axisymmetric model
Thank you for sharing this. The suggestions look promising, I will try them and let you know
i took simplified models for testing, even the mesh during deformation is not highly distorted, still the analysis divergences (half below of prescribed displacement). As previously guessed, the problem may occur due to residual stress for next iteration at the corner region.
some questioning is in rounded corner, previously shown not help. Interesting me to try and reproduces.
This looks interesting. I think these high stresses are occuring because of large deformations of the parts which are compressed between two metal parts and can not deform anymore
probably right, similar to 3d metal forming analysis i still stuck in converge issue even try many problems setting and mesh preparation. Latest nonlinear algorithm solver in CalculiX by Newton-Raphson, Riks or Arc length which may help is not yet available.
Hi,
I’m focusing on why some of my elements fail while others apparently under similar conditions don’t.
I have done some tests, and this particular result would be breaking the rotational invariance of the solution.
Four Hyperelastic cubes. All nodes fixed except the ones in one edge which are displaced inwards to make the element collapse (imposed displacement). Two of the cubes accommodate the volume properly while the other two show a strange deformation pattern. Could this be just a graphical glitch issue?
¿What do you think?
Regards
Fixed nodes
Imposed displacement inward while third DOF is free.
Deformation. True Scale.
Can you share the .inp file ?
Yep.
*NODE
1,0,0,0
2,0.001,0,0
3,0.001,0.001,0
4,0,0.001,0
5,0,0,0.001
6,0.001,0,0.001
7,0.001,0.001,0.001
8,0,0.001,0.001
9,0,-0.002,0
10,0.001,-0.002,0
11,0.001,-0.001,0
12,0,-0.001,0
13,0,-0.002,0.001
14,0.001,-0.002,0.001
15,0.001,-0.001,0.001
16,0,-0.001,0.001
17,0,-0.004,0
18,0.001,-0.004,0
19,0.001,-0.003,0
20,0,-0.003,0
21,0,-0.004,0.001
22,0.001,-0.004,0.001
23,0.001,-0.003,0.001
24,0,-0.003,0.001
25,0,-0.006,0
26,0.001,-0.006,0
27,0.001,-0.005,0
28,0,-0.005,0
29,0,-0.006,0.001
30,0.001,-0.006,0.001
31,0.001,-0.005,0.001
32,0,-0.005,0.001
*ELEMENT,TYPE=C3D8R
1,1,2,3,4,5,6,7,8
2,9,10,11,12,13,14,15,16
3,17,18,19,20,21,22,23,24
4,25,26,27,28,29,30,31,32
*NSET,NSET=T1
3
7
17
21
*NSET,NSET=T2
10
14
28
32
*ELSET,ELSET=2
1
2
3
4
*MATERIAL,NAME=MOONEYRIVLIN
*HYPERELASTIC,MOONEY-RIVLIN
388400,97100,6E-08
*SOLID SECTION,ELSET=2,MATERIAL=MOONEYRIVLIN
*TRANSFORM,NSET=T1
0.7071067811865,-0.7071067811865,0,0.7071067811865,0.7071067811865,0
*TRANSFORM,NSET=T2
0.7071067811865,0.7071067811865,0,-0.7071067811865,0.7071067811865,0
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
2,1,,0
2,2,,0
2,3,,0
4,1,,0
4,2,,0
4,3,,0
5,1,,0
5,2,,0
5,3,,0
6,1,,0
6,2,,0
6,3,,0
8,1,,0
8,2,,0
8,3,,0
9,1,,0
9,2,,0
9,3,,0
11,1,,0
11,2,,0
11,3,,0
12,1,,0
12,2,,0
12,3,,0
13,1,,0
13,2,,0
13,3,,0
15,1,,0
15,2,,0
15,3,,0
16,1,,0
16,2,,0
16,3,,0
18,1,,0
18,2,,0
18,3,,0
19,1,,0
19,2,,0
19,3,,0
20,1,,0
20,2,,0
20,3,,0
22,1,,0
22,2,,0
22,3,,0
23,1,,0
23,2,,0
23,3,,0
24,1,,0
24,2,,0
24,3,,0
25,1,,0
25,2,,0
25,3,,0
26,1,,0
26,2,,0
26,3,,0
27,1,,0
27,2,,0
27,3,,0
29,1,,0
29,2,,0
29,3,,0
30,1,,0
30,2,,0
30,3,,0
31,1,,0
31,2,,0
31,3,,0
*AMPLITUDE,NAME=A_3
0,0
1,0.001
*AMPLITUDE,NAME=A_4
0,0
1,0.001
*AMPLITUDE,NAME=A_5
0,0
1,0.001
*AMPLITUDE,NAME=A_6
0,0
1,0.001
*STEP,NLGEOM=YES,INC=110,AMPLITUDE=STEP
*STATIC,SOLVER=PARDISO
0.01,1,0,0.01
*BOUNDARY,AMPLITUDE=A_3
3,2,,-1
*BOUNDARY,AMPLITUDE=A_3
7,2,,-1
*BOUNDARY,AMPLITUDE=A_4
10,2,,1
*BOUNDARY,AMPLITUDE=A_4
14,2,,1
*BOUNDARY,AMPLITUDE=A_5
17,2,,1
*BOUNDARY,AMPLITUDE=A_5
21,2,,1
*BOUNDARY,AMPLITUDE=A_6
28,2,,-1
*BOUNDARY,AMPLITUDE=A_6
32,2,,-1
*NODE FILE,GLOBAL=YES
U,RF
*EL FILE
S,NOE,E,ENER
*END STEP
Interesting. When submitting it in Abaqus, I sometimes get the following errors:
***ERROR: Invalid nodal coordinate values were specified for the following
nodes: 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23
24 25 26 27 28 29 30 31 32 33 34
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
INTERPRET SOME DATA. SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION
***ERROR: in keyword *HYPERELASTIC, file "test_abq_3.inp", line 95: OdbError:
Tabular data for at least one option or suboption has
either blank or zero valued row(s).
while sometimes (without changing anything) it completes and here are the results:
If the .pmx file can be shared, I can take a look if there is a graphical problem.
Abaqus shows the same so it shouldn’t be the case. There might be something wrong with the definition (nodal connectivity) of those elements.
The displacements at the nodes look the same, don’t they? Do you mean those blue triangles? That looks like what happens when you draw a concave square using two triangles.
HI,
I have cleaned the model as there was two orphan nodes with intercalated numbering. Just in case. I guess connectivity is right but it shows the same behavior.
VM is the same but Sxy and deformation is different.
I edited the previous post with the new inp and corrected the description as this is not breaking the symmetry under rotation but breaking the rotational invariance of the solution. Sorry.
Any idea why there is delivering different solutions. ? ?