Compression test (static nonlinear)

I am new in simscale and trying to perform my first simulation.
It is a compression test with strain rate 0.002 s^-1 and the nature of this project is static nonlinear. I want to have a force vs. displacement graph from the simulation. But every time I run, the simulation failed. It is probably due to improper simulation set up.
Can anyone help me regarding this?

Protective Structure - Quasi static compression simulation | SimScale Workbench

1 Like

Hi, and thanks for using the forum!

My usual approach in this case is to switch from the force-driven simulation to a displacement-driven one. The problem is that you need to leave the Z displacement unconstrained, and sometimes the physical contact is not enough at first step to constrain the part.

To obtain the force curve, add a Result control item - Area - Sum - Reaction force to the face were you apply the displacement.

Please try this approach and let me know if you need further help.

1 Like

Thanks for your response.
I have tried with the instructions but it failed. Displacement boundary condition is applied but I don’t know how to make the Z displacement unconstrained. Should I apply remote displacement? I also tried with this and showed the model is overconstrained.
However after running simulation this error message showed up:

Protective Structure - Quasi static compression simulation | SimScale Workbench

Please perform these changes and try again:

  1. Assign the fixed value BC to the top face and not to the one under contact.
  2. Under ‘Numerics’, change the ‘Convergence criteria’ to ‘Absolute’
1 Like

Thank you .
The simulation runs successfully.
I get the force vs time curve but desire to get the force vs displacement curve. Would you tell me how can I get that?
Moreover, the colored picture shows that there is stress on the upper platen but I want it as a rigid body so that no rigid body motion (interpenetration) occurs during the simulation. How can I ensure that?
Although this is a nonlinear static analysis, I define the ABS material as linear one since to define it as ‘elastoplastic’ I need the true stress strain data. And I failed to collect any such type of data for ABS. Would you tell me how can I get that?
Protective Structure - Quasi static compression simulation | SimScale Workbench
Please pardon me for asking so many questions!

Don’t worry, we are here to help!

You applied the displacement in the wrong direction, please fix and try again.

1 Like

Thanks. The direction is fixed now. In the x-axis it shows time value but I want replace it with displacement. Would you suggest any way?
Can I have the plastic deformation region in the same plot along with the linear elastic region?

Protective Structure - Quasi static compression simulation | SimScale Workbench

You can create this plot locally by downloading the result curves in CSV format, and use a program to process it. For example a spreadsheet software, Python, Matlab, etc

Thanks for the idea. I have drawn the force vs displacement curve but it only shows me the linear region. Can I get the plastic deformation region in the curve?

Yes, you can get the plastic region from the curve if you:

  • Assign an Elasto-Plastic material
  • Apply a displacement that is large enough to cause the plasticity to develop

Please refer to the documentation for details on how to specify such material.

If I want to get a stress-strain plot should I go through the same way as the reaction force i.e. Result control>Area calculation>Sum>Stress/Strain?
According to my simulation which one should I use “Area calculation or Volume calculation”?

It depends on what you want/need.

I think that for an stress/strain plot to make sense, you must sample the quantities at the same point. You can do that with a Result control item - Point Data.

1 Like

Would you tell me, what is the difference between nodal force and reaction force in face calculation?
If I consider the force required to deform the structure which one should be calculated?
While selecting point data for strain, I found two strain i.e. total nonlinear strain and equivalent plastic strain, if want to plot the stress-strain curve which one should be selected?

Hi again!

Reaction forces only appear on faces with constrained displacement (fixed value or fixed support), while nodal forces also appear under other conditions such as loads, contacts, etc.

With the displacement-driven simulation, you should measure the reaction force on the faces where the displacement is imposed. For this use a Result control item - Surface data - Sum - Reaction force.

For the strains, the equivalent plastic strain only appears on elasto-platic materials, and when the yield condition is reached. I couldn’t tell what strain you need, any of them should be viable in different situations.

Thank you for your continuing support.

Although defining the material as a nonlinear one, the reaction force is still linear. Would you tell me how to get plasticity in the force curve?

Actually, I want the stain that is generated due to the von misses stress. In this case which one should I choose to plot the stress-strain curve?

Protective Structure - Quasi static compression simulation | SimScale Workbench

As your case is unidirectional compression, I would measure the stress and strains in the load direction:

  • A few point data control items, in different locations
  • Strain would be EPZZ (z normal strain, vertical direction) from field Total Strain
  • Stress would be SIZZ (z normal stress, vertical direction) from Cauchy Stress

If you do not see the plastic region, perhaps your load is not enough to achieve it.

1 Like

Thanks, your reply dispels my confusion!

I have just copied the simulation and defined a custom material (polyvinyl alcohol sponge) as hyper elastic. But while running the simulation it shows the failure message. Do you have any suggestion for me on how to overcome this?

Displacement controlled uniaxial compression simulation | SimScale Workbench

However, there is a limit of 10 simulations in the community plan and I have already ran 6. After 10 is it auto renewable or I can’t run any even though have enough core hours?

I also tried with the linear elastic model of the material and it failed too.

I can not understand what mistakes I have done, please help.
Displacement controlled uniaxial compression 2 | SimScale Workbench

Thanks @ggiraldof, your replies really help me to understand and grow insights on this kind of project.


I think that the D1 parameter might be too low, please increase to something around 1e-6 ~ 1e-8. By the way, where did you get the parameters from?

I am sorry yes, after 10 successful runs the community plan expires. You can for example apply to the academic program, if you have are currently enrolled as student:

What other changes did you perform?