Von Mises vs PEEQ

Hi!,
I am modeling a dent in a pipe using a compressive force distributed over a region of the external surface of the pipe. I use an elasto-plastic model with geometric nonlinearity, static analysis and C3D20R elements. I note that the value of the equivalent plastic strain PEEQ does not agree with the Von Mises stress value in the stress-strain curve of the material. That is, for the SVM stress shown in the figure (~90000 Psi), a PEEQ value of 0.26 must be showed, according to the stress-strain curve of the material. However, a value of 0.0357 appears. Is this correct? Could it be a convergence problem?

Thanks in advance,

Jack

Loooking at the manual, it says:

PEEQ [PE]: equivalent plastic strain.

That suggests it does not include the elastic strain.

Try looking at ME instead.

1 Like

That’s the full stress-strain curve but in CalculiX you have to input stress vs plastic strain data. Also, keep in mind that the values might be different due to extrapolation. To avoid that, you should check the integration point values in the .dat file (request them using *EL PRINT).

1 Like

Hi Juseche,

¿ Would you mind sharing the source of those stress-strain values shown on your curve for API 5L X52 ?

This is why I ask. there are different sources out there.

Figure 1. True stress–strain curve for API 5L X52, X65, and X80 steel pipe [5,7,20].

  1. Lo, M.; Karuppanan, S.; Ovinis, M. Failure Pressure Prediction of a Corroded Pipeline with Longitudinally Interacting Corrosion
    Defects Subjected to Combined Loadings Using FEM and ANN. J. Mater. Sci. Eng. 2021, 9, 281. [CrossRef]

  2. Belachew, C.T.; Ismail, M.C.; Karuppanan, S. Burst strength analysis of corroded pipelines by finite element method. J. Appl. Sci.
    2011, 11, 1845–1850. [CrossRef]

  3. de Andrade, E.Q.; Benjamin, A.C.; Machado, P.R., Jr.; Pereira, L.C.; Jacob, B.P.; Carneiro, E.G.; Guerreiro, J.N.; Silva, R.C.; Noronha,
    D.B., Jr. Finite element modeling of the failure behavior of pipelines containing interacting corrosion defects. In Proceedings of
    the 25th International Conference on Offshore Mechanics and Arctic Engineering—OMAE, Hamburg, Germany, 4–9 June 2006;
    pp. 315–325. [CrossRef]

Thanks

MPC model of API-579-2021. Here (I’m using ccx2.13):

** material definition
*MATERIAL, name=mat
*ELASTIC
2.940000e+07,0.260000,0
*PLASTIC,HARDENING=ISOTROPIC
52000,0.000,0
54876,0.018,0
57751,0.036,0
60627,0.053,0
63502,0.071,0
66378,0.089,0
69253,0.107,0
72129,0.124,0
75004,0.142,0
77880,0.160,0
*SOLID SECTION, ELSET=Eall, MATERIAL=mat
**

Thanks

Jack.

in this table real stress (PSI) and real strain (in/in).

*STEP, NLGEOM,INC=10000
*STATIC
0.000010,2.000000,1.000000e-08,0.010000

Jack.

Thanks for your answer.
Yes. Indeed, plastic yield iniciated at stress values above of Sy witn peeq values not according with strain-stress curve value.

Jairo

Thanks for your answer.

Yes I reviewed *dat file, but Indeed, plastic yield iniciated at stress values above of Sy witn peeq values not according with strain-stress curve value.

Jack

Yes. Indeed, plastic yield iniciated at stress values above of Sy with peeq values not according with strain-stress curve value.

Jairo

It works fine to me.

Have you tried with ccx v2.21?

¿Could you temporarily remove the temperature dependency from the curve?.

I see.

Could be a problem related with time step?

Which element, among c3d20 and c3d20 with full o reduced integration, works better for finite plasticity with large displacement problems?

Any recomendation about meshing with c3d20 and c3d20?

I’m have a problem installing ccx 2.21 in Ubuntu >20.04, because libgfortran4.so is not available. What can I do?

Thanks for your help!

Second-order full integration elements are not recommended for problems involving large plastic strains (due to volumetric locking). You should use reduced integration elements instead.

Seems too much deviation to me. Do you ramp the load ¿right?
Could you post the full inp.?

Regarding geometry :

I always prefer to start with coarse parabolic elements with nodes on geometry, specially for circular shapes. In case I need to refine or move to linear nodes remain on top of geometry.

Regarding element performance

I’m thinking there is another option to consider.
Even if the model is a unique component all made of API 5L X52, one doesn’t necessarily need to define plasticity everywhere ¿isn’t it?.
Not sure if this may boost the analysis as NLGEOM will be activated anyway. ¿What do you think?.
At least one would be freer to choose different element formulations far from yielding areas.

I think that I wouldn’t risk this approach since, apart from local yielding, there’s also global stress redistribution due to plasticity.

But there is no plasticity below the yield point. Outside the yield area (being conservative when defining it) material could be defined as linear elastic. ¿isn’t it?.
With one final check on VM to see if the assumption was correct.
I’m considering the paper JMSE | Free Full-Text | Empirical Failure Pressure Prediction Equations for Pipelines with Longitudinal Interacting Corrosion Defects Based on Artificial Neural Network as example .It might be similar to Juseche problem.

In that case there is no need to define plasticity everywhere. The yield area is well defined arround the defect.

Thanks for your answers,
I managed to control the high stress levels quite a bit by using a complete model of the pipe instead of using symmetry conditions. I noticed that the high SVM values ​​not related to PEEQ occurred in the symmetry plane (see figure in my first post) where the bending effects are most pronounced. However, I’m still not entirely convinced of the results.

Please tell me, how to attach the *INP file of the model (I don’t see options for this here).

Regards

Jack

If it’s rather short, you can paste it here using the “Preformatted text” option. If it’s not so short, upload it to some hosting website like Google Drive, Dropbox or WeTransfer and paste the link here.

Here:

Thanks

Jack

I don’t use google drive. Could you post it via we-transfer