Problem with material definition 1

[jj89]

Dear people,

Any idea how I could solve this problem ????

When I submit my .CAE appears this Error ...
-----------
Failed to regularize material data for material ALUMINIO. Please check your input data to see if they meet both criteria as explained in "MATERIAL DATA DEFINITION" section of Abaqus Analysis User Manual. In general, regularization is more difficult if the smallest interval defined by the user is small compared to the range of the independent variable.
-----------

I don't know what could be happening...

For further data, just ask to me and I reply what ever!!

Thank you !!!!!

 

[StefCon]

Hello,
I read about this recently.

Link

"When performing an analysis, Abaqus/Explicit may not use the material data exactly as defined by the user; for efficiency, all material data that are defined in tabular form are automatically regularized. Material data can be functions of temperature, external fields, and internal state variables, such as plastic strain. For each material point calculation, the state of the material must be determined by interpolation, and, for efficiency, Abaqus/Explicit fits the user-defined curves with curves composed of equally spaced points."

You are running explicit, right? Maybe removing some data points or adding some to get a more even spacing (or larger spacing) could help. Just a guess.

Good luck!

 

[akabarten]

Hi,

For some performance reasons Abaqus does not use exactly material points you defined in model.

Explanation of the topic you will find here:
Getting Started with Abaqus: Keywords Edition, 10.2 Plasticity in ductile metals, Data regularization in Abaqus/Explicit.

To overcame the problem you can:
- change regularization tolerance (can be done with specific material types)
- completely turn off regularization (can be done with specific material types)
- add/remove material points in you material definition (should work always)

Regards,
Bartosz



VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[jj89]

Hi!!

Thank you, I tried to remove intermediate poinst and also i tried to put more points but alwais apear the same error... Also I didn't find "specific material types".

I dont know what happen, if somebody can have a look to my CAE would be great!!
I attached the document.

Regards,
Juan

 

[StefCon]

Hello,
I tried it. The strain values you defined are not correct I guess. The steels I work with has a plastic strain max at maybe 0.15-0.18 (aluminium should not be too far off). Also, check the unit for the youngs modulus. The plastic stress values are in MPa I assume. Youngs for alu ~ 70 000 MPa.

I divided your strain values with 1000 to make them in the "normal" range.
I also removed the first data point (45,0) and the analysis finished the pre-check. It didn't start however. See error message below.

Best regards,

The rigid bodies with the reference nodes contained in node set ErrNodeRefNodeNoMass have no mass associated with them and some degrees of freedom of the reference node are not restrained. Either mass must be defined or all of the translational degrees of freedom must be constrained. See the status file for further details.

*Plastic
95., 0.
195., 0.010861
215., 0.022678
255., 0.078599
275., 0.134219
285., 0.172401
295., 0.219193
305., 0.276072
315., 0.344695
325., 0.426916
335., 0.524794
345., 0.640614
355., 0.776897
365., 0.936421
375., 1.12223
385., 1.33766
395., 1.58636
405., 1.87227

 

[jj89]

yes.. sorry, i forgot to look for the young, the idea is to to simulate hot aluminium and i found for 480ºC it is about 32200 Mpa and aldo I am not sure how to obtain data for plastic area, I just sow from a grafic it is start in about 50 MPa but the rest of the data i'm not sure, I'm using Ludvik law with n=0.17, K=400 and fluence stress 50, Any body has a better source to get a good data?