Strange results for the 2D plane stress

General Questions
1

Hello Community,
(I apologise for the bad English; I am using a translator).
I am a civil engineer, of a certain age, in Italy (freelancer) very fond of advanced FEM modelling. I must say that there was a real need for a pre and post processor for Calculix, and for this goes all my admiration for the creator of Prepomax. Thanks for the work done will never be enough. Acknowledgements that should certainly also be extended to the disseminators who patiently produce excellent tutorials. In this regard, I followed with interest those made available by user “FEAnalyst” on youtube. In particular, I have also tried to replicate (using his geometric file made available) the example in Tutorial 16, it is the study of an object subjected to a plane state of tension and the modelling is done with shell-section elements. This is where something started to confuse me as I was expecting that for S33, S13 and S23 the value of the stresses would be zero while the results give me non-negligible values when compared to S11, S22 and S12. Where did I miss out? S33, S13 and S23 are null only if I assign the poisson coefficient the value zero. Furthermore, out-of-plane displacements (U3) are also not zero, it’s very strange.

Thank you for your attention

2

Thanks, I’m glad that you like my tutorials. Unfortunately, CalculiX doesn’t have true 1D and 2D elements - they are always expanded to 3D elements internally and that’s why such effects occur: Discrepancy in Element Stiffness Matrix Output using Substructure Approach - #29 by vicmw - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).

So you can only ignore them or play with material properties, as you’ve mentioned.

3

Thank you for taking the time. The argument is that even if you ignore them, they actually affect Von Mises’ tension, so perhaps it is better to ‘play’ on the properties of materials. But this can be a solution for simple models. Then the argument would extend to2D plan strain problems with some extra difficulty in assigning material properties so that epsilon(z)=0. Anyway, I’m glad I wasn’t completely wrong

4

Seems the problem is really with the plane stress and plane strain idealizations while CCX uses a more correct model, isn’t it?

5

We had some debate about this and some possible workarounds where discussed.
You could try it and compare with some other software as reference.

The idea is to define the material as Orthotropic to remove the S33 component and make it Plain Stress compliant.

imagen
imagen1176×624 144 KB

EDITED: Removed the OUTPUT 3D option to avoid confusion. I’m Using CPS8R

imagen
imagen1247×739 127 KB

imagen
imagen1216×742 98.1 KB

6

Thank you. Sorry to take advantage of your availability… Have you had a look at the U3 displacements? Are they zero? Because in the initial problem, the U3 displacements were also significant

7

They are essentially (just not exactly - numerics) zero in my original model:

U3
U3968×694 91.8 KB

Modified material gives exact zero:

U3 v2
U3 v21054×693 70.7 KB

8

Good morning,

Some time ago, I had the same problem, and it was due to the fact that the ENGINEERING CONSTANTS entry requires the orientation of the material’s orthotropy to be specified; an example would be the following:

*MATERIAL,NAME=ECMATERIALEUCALIPTO
*ELASTIC,TYPE=ENGINEERING CONSTANTS
18000000,20000000,18000000,0.20,0.25,0.20,11250000,13333333,
11250000,0

*DEPVAR
10

*Orientation, Name=orientationX, System=RECTANGULAR
1.,0.,0.,0.,1.,0.
*Orientation, Name=orientationY, System=RECTANGULAR
0.,1.,0.,0.,0.,1.
*Orientation, Name=orientationZ, System=RECTANGULAR
0.,0.,1.,1.0,0.,0.

Until then, the models were convergent, but the results were incoherent. I admit that I have not conducted tests with shell models, but perhaps this condition could be helpful.

Best regards
Damian

9

Clearly I was referring to the exercise I did on the original geometry. If they had been results of the order of E-10 I would certainly have considered them null.
Anyway thank you all, now the problem is much better understood

10

I recall doing some checks and results where OK . Did you try some problem with known solution to be sure your inputs where right.?.

EDITED: There were no thermal expansions involved.

11

Sorry for the delay in my response; to check the functionality of the ENGINEERING CONSTANTS keyword, I prepared a model with a linear elastic material and, in parallel, an ENGINEERING CONSTANTS material with the three constants similar in the three directions and of a value similar to the first one. Apparently, unless I am mistaken, the both should lead to results that are not exactly the same but practically identical. Far from it, the results were really different.

I saw this thread on the forum referencing the *ORIENTATION and the ENGINEERING CONSTANTS keyword:

Once the *ORIENTATION keyword was introduced, the two models yielded practically similar results, which, from my point of view, was expected.I need to conduct many tests in this regard, but it seems like a good approach to simulate the behavior of wood in PrePoMax. I hope my comment has been helpful.