Difference between TOSTRAIN, MESTRAIN and PE

General Questions
1

Good evening, I do not fully understand the difference between TOSTRAIN, MESTRAIN and PE in results: can you please explain me the difference or point me out some references where I can find informations?

Thank you!

2
  • TOSTRAIN - total strain (mechanical including elastic and plastic + thermal)
  • MESTRAIN - mechanical strain (elastic and plastic)
  • PE - plastic strain
2 Likes
3

Thank you for the exhaustive answer: in the meantime I ran a coupled temperature-displacement simulation, using temperature dependent material properties. Although TOSTRAIN reach values of 0.67 PE still is 0 for each step and each calculus iteration (NLGEOM is ON).

The material I am analysing is a PBT (Polybutylene Terephthalate), for which I provided stress-strain curves for different temperatures in the plastic regime, as well as different elastic moduli at differen temperatures.

Am I missing something?

4

Do the stresses exceed the yield strength of the material ? Did you define plasticity starting from yield strength and zero plastic strain and then adding more true stress vs true plastic strain points ?

5

Yes, stresses exceed yield strenght: I defined material curves as you described, starting from yield and zero plastic strain, up to ultimate stress. first point in material curve is 33MPa, I reach 142 MPa.

6

What if you remove all temperature dependencies, thermal BCs / loads and run a purely mechanical analysis ?

Can you share the file ?

7

Unfortunatelly I cannot share the model due to intellectual property restrictions. I did further analyses:

  1. coupled thermo-mec. analysis, same material (temp. dependent, without deleting material properties at different temperatures), at one specific temperature → PE=0
  2. coupled thermo-mec. analysis, same material (temp. dependent, deleting material properties at different temperatures other than the one used in analysis), at one specific temperature → PE=0
  3. coupled thermo-mec. analysis, mec. prop. independent from temperature, at one specific temperature (it should be the same as a pure mechanical analysis) → PE=0
  4. static analysis, mec. prop. independent from temperature, → PE up to 0.49

Here some screenshots of analysis 2,3 and 4:

Analysis 2 (auto-def is ON)

image
image644×703 134 KB

Analysis 3 (auto-def is ON)

image
image644×703 135 KB

Analysis 4 (auto-def is ON)

image
image644×703 139 KB

Between analysis I didn’t change anything, I created analysis cases inside the same model.

8

So just changing the step type from coupled temperature-displacement to static results in PE ≠ 0 ?

You could compare the input files after exporting to make sure that’s the only difference.

I made a single element test and I get non-zero PE with this kind of step and temperature dependence. Maybe try playing with it and adding features from your model to see if it still works:

PE temp test.pmx (36.5 KB)

1 Like
9

I found out what I was doing wrong! Since I was interested only in thermal expansion of component, I didn’t define specific heat and thermal conductivity, turns out it is essential to have PE in results!

1 Like
10

Good to know. CalculiX often just fails without errors or doesn’t provide some results without warnings when something is missing in the setup.