C3D8I fails patch test

1

This element does work much better than C3D8 in many cases but an important one it doesn’t is the MacNeal-Harder patch test. From what I understand, that implies it won’t always converge to the correct solution with mesh refinement. I wonder if anyone has any thoughts on whether this is safe to use as a general replacement for C3D8, which does pass the patch test but of course performs badly in bending. CCX 2.10 and 2.21 both have the same results so it’s not related to the change Guido proposed here C3D8I-Element in CalculiX

C3D8I patch test solution

MacNeal-Harder patch test
MacNeal-Harder patch test656×886 42.3 KB

*NODE
1,0.249,0.342,0.192
2,0.826,0.288,0.288
3,0.85,0.649,0.263
4,0.273,0.75,0.23
5,0.32,0.186,0.643
6,0.677,0.305,0.683
7,0.788,0.693,0.644
8,0.165,0.745,0.702
9,0,0,0
10,0,1,0
11,1,1,0
12,1,0,0
13,0,0,1
14,1,0,1
15,1,1,1
16,0,1,1
*ELEMENT,TYPE=C3D8I,ELSET=DEFAULT
1,1,2,3,4,5,6,7,8
2,1,4,3,2,9,10,11,12
3,5,6,7,8,13,14,15,16
4,1,2,6,5,9,12,14,13
5,2,3,7,6,12,11,15,14
6,3,4,8,7,11,10,16,15
7,4,1,5,8,10,9,13,16
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
1000000,0.25
*SOLID SECTION,ELSET=DEFAULT,MATERIAL=MATERIAL
*STEP
*STATIC
*BOUNDARY
9,1,,0
9,2,,0
9,3,,0
10,1,,0.0005
10,2,,0.001
10,3,,0.0005
11,1,,0.0015
11,2,,0.0015
11,3,,0.001
12,1,,0.001
12,2,,0.0005
12,3,,0.0005
13,1,,0.0005
13,2,,0.0005
13,3,,0.001
14,1,,0.0015
14,2,,0.001
14,3,,0.0015
15,1,,0.002
15,2,,0.002
15,3,,0.002
16,1,,0.001
16,2,,0.0015
16,3,,0.0015
*EL FILE
S,E
*END STEP
2

Hi, should we avoid using this element for the moment?. It seems to affect the results appart from convergence.

3

I hope not. It’s more accurate than C3D8 in just about every test I’ve done. I also tried making a mesh filled with trapezoids and it wasn’t very good. But this is pretty artificial - usually when you refine anything, the elements morph towards parallelepipeds which seem to be fine.

Stress XY should be 1 MPa

C3D8I weirdness
C3D8I weirdness1760×1344 136 KB

2 Likes
4

The same input file submitted in Abaqus:

abq patch
abq patch750×598 12.1 KB

5

I just checked the integration point values for C3D8 and C3D8I

C3D8
image

C3D8I
image

Basically each row in a column should have the same value. That’s not happening for C3D8I.

Could anyone check the integration point values in abaqus?

6

No need to check with Abaqus, they should be equal as you say.

1 Like
7

it has been submitted the bugs of linear hexahedral (incompatible) element at specific case of distorted mesh. In the past, i have given an example of concentrated stress in plate with a hole, unfortunately there’s no improvement for every new release of CalculiX versions. Element and results still perform better for structured mesh and less distorted than linear ones.

8

Has the proposal already been implemented? His post was from Nov 2021, the last change of C3D8I elements according to the LOGBOOK was in Oct 2021.

2 Likes
9

Hopefully that change was the fix and just needs plugging in! I’ve tried to contact Otto Bernhardi by guessing his email address but no reply.

1 Like
10

it has known good and better at coarse mesh reported by the author, but not any notification available for distorted mesh. Probably a different element formulations with previously, more testing is needed.

11

The paper it’s based on is specifically an update that’s meant to work with distorted elements. I’ve implemented a very similar one (maybe the same one) myself and it’s fine for moderate distortions like this or what you’d get around a circular hole.

12

Hello,

A long ago I recall someone pointing that C3D8I elements couldn’t be used in *DYNAMIC calculations.

I have been searching about it and I can only find warns about two points:

-Using C3D8I element subjected to torsion and
-Sometimes, discrepancies when Vibration modes and frequencies are required.(I guess if discrepancies show up when there are torsional modes involved)

Is there something fundamentally wrong about using C3D8I with Dynamics if they do not require a previous *Frequency card or involve torsion.?

Thanks

13

In Abaqus, incompatible mode elements are really versatile, considered as general-purpose and usable in large strain problems. They eliminate shear locking, don’t have hourglass modes and don’t exhibit volumetric locking for nearly incompressible behavior (full incompressibility requires hybrid elements). They work well with plasticity and contact except that convergence might be slower when large plasticity is involved. They may also fail to converge with hyperelasticity, especially when significantly distorted. By the way, they are prone to distortion, their performance is worse for elements with a parallelogram shape and much worse (to the point of uselessness) for a trapezoidal shape. However, they can also be used in dynamics and impact problems. But in Abaqus, they pass the patch test…

1 Like
14

SAP finite element programs use incompatible element as a default and replacement (no standard is provided), it’s use for static and dynamic analysis (Wilson and Ibrahimbegovic, 1990).

15

Thank you both for the information and references.
If I find any glaring weaknesses I will report.

1 Like