Wrong force values

[catrueeb]

I have tried to validate my model with a some tests but it seems that the Total Contact Force values of my simulation are around 40% different from the real values. I am using a hyperelastic Ogden model with NLgeom on, linear mesh elements and no friction. Where is this discrepancy coming from? Is it a mistake I am missing or is it normal the force values are not corresponding to real values?

 

[Mustaine3]

The error could come from a lot of things you've done. Material data, element type, procedure, load, BC, postprocessing...
You have to question everything and check it.

 

[catrueeb]

Ok yes I did this. If you do everything right, can you relate contact force values of FEA simulation to real test force values? Should they be the same? Of course if you have a good material model.

 

[Mustaine3]

Yes, if you do everything right, then the result typically match very closely.
But in my experience a lot of users don't do everything right.

 

[Dave442]

How are you extracting/summing the contact forces?

 

[Mustaine3]

Output variables CFN and CFS could be used.

 

[catrueeb]

Thank you for the answers. I feel quite confident about my model... Few facts:
Output variable: Total contact force CFN
Contact Type: Normal / node to surface / very fine slave mesh
Displacement Controlled
Material: Ogden model from 3 different types of stress/strain tests --> no other material parameters
Hybrid Linear Elements

It seems the material is stable, the problem is converging... But the error still is quite big.

 

[Dave442]

A couple of suggestions:

CFN is total contact force due to contact pressure. CFS is total contact force due to friction, and CFT is total contact force due to CFN + CFS. Are you looking at the right output variable? Is friction a factor in your test?

Also, i think CFN and CFS are resultant quantities. So if there are nodes on your contact surface that have force components acting in opposite directions they will cancel. You can extract/sum field output CNORMF and CSHEARF if this is an issue.

Also worth looking at CNAREA to see does it match your test. I'd also try surface-to-surface contact if contact output is of interest. Are your FEA results 40% higher or lower than your test?

 

[catrueeb]

Hi Dave442 and sorry for my late response

We are neglecting friction in our tests, but I have also tried including friction and it does not change much of the normal force.
My test values are SMALLER than my simulation values.
I am already using a very fine slave mesh for my contact, therefore changing to surf-surf contact also does not change a lot.
I do not think it is a problem in my case to use resultant quantities... I am only looking at the normal force value in z-direction. So in case there would actually be any force in (minus)-z direction, I would need to include it as well.
We are fitting the model parameters using unibiaxial & equibiaxial tests, but maybe it is just not possible to get accurate values for difficult force distributions?

Regards

 

[Dave442]

if you're confident in your analysis and your output I would query the test data:

was material processing and/or pre-conditioning taken into account?
were temperature and rate effects taken into account?
could the materials have anisotropic properties?
was the hyperelastic material model defined correctly?
have you verified FEA stress-strain data vs. test data for your different deformation modes?

 

[catrueeb]

Thank you for your answer.
Aging, temperature, rate dependency and other effects were considered. Also I think there is no large anisotropic behaviour.
Hyperelastic material: I tried two different definitions of the Ogden model, both led to the same results.
I have not verified my stress-strain data, I got the data from a material scientist. How would you do this? Simulate the material tests in Abaqus?

Regards

 

[Dave442]

i create a single element and verify the stress-strain output matches the test data for each deformation mode (uniaxial, biaxial etc.).

this verifies the defined correctly and behaving as expected. if the FE output doesn't match test data something may be defined incorrectly.

Abaqus has a "material evaluation" tool that will do all this for you automatically. This is demonstrated in the documentation:

Getting Started with Abaqus Interactive Edition -> 10 Materials -> 10.7 Example: Axisymmetric Mount