Negative Jacobian Error: Viscoporoelastic Indentation Mesh Sensitivity Analysis

[moon]

Hello

I created a viscoporoelastic spherical indentation model with a quarter symmetry.
The idea was to conduct a mesh sensitivity analysis and observe how and if the result would change for finer or coarser meshes. The other parameters were kept unchanged. However, when doubling the elements of the model or dividing them by e.g. 1.5 times, the model does not terminate normally anymore. The error occurring is: Negative Jacobian.

‘Default’ model parameters:
- indenter radius: 0.5mm
- tet4 elements for indenter: 1831
- linear hex elements for sample: 13875
The mesh was created in ABAQUS and then imported in FEBio.

- biphasic contact formulation
- indenter: rigid body (impermeable)
- sample:
E: 5 kPa
v: 0.075
k: 1.7e-2
gamma1: 1.844
tau1: 58
- force-controlled

- laugon: ON
- tol: 0.01
- gaptol: 1e-6
- penalty: 10
- two_pass: Off
- auto_penalty: On

Afterwards, I tried it with penalty = 1 and set the tolerance down to 0.0001. But the model did not converge yet. Unfortunately, the model exceeds the limit for the upload.

I would be very thankful for inputs how to adapt the parameter and what could cause this behaviour.

Moon

[ateshian]

Hi Moon,

You can try importing the refined model file into PreView and using the Mesh Inspector tool to see if there are any inverted elements in the mesh. If so, it could be that the mesh refinement step in ABAQUS was at fault.

Best,

Gerard

[moon]

Hi Gerard,

thank you for the adivce.
Attached you find an overview of the information from the mesh inspector for the three models.

Best,

Moon

[ateshian]

Hi Moon,

So there doesn't appear to be a problem with the mesh at the outset. Can you provide the log output for your model that fails?

Best,

Gerard

[moon]

Hi Gerard,

attached you find the log files for the two simulation with penatly1 and penalty10 and one time for tol=0.0001.

Best,

Moon

[ateshian]

Hi Moon,

I suggest that you turn off the tolerance (tol=0) and increase the gap tolerance (gaptol=1e-3), since you are using units of mm and gaptol of 1e-3 would be 1 micron (for a sphere radius of 0.5 mm), which is very tight. I also suggested that you switch from Broyden to full Newton (max_updates=0, max_refs=25).

Please try that and let me know if it improves things.

Best,

Gerard

[moon]

Dear Gerard,

thank you very much for this valuable input.
The simulation with twice as many elements seem to have normally terminated now.

Best,

Moon

[weiss]

Hi Moon,

You are using the augmented Lagrangian method. Did you try running the analysis with this feature turned off (laug=0)?

You have tolerances set for both tol and gaptol, and gaptol is set very tight:

- laugon: ON
- tol: 0.01
- gaptol: 1e-6

Note that gaptol has units of length, i.e. 1e-6 mm.

Also, it appears that you don't have the auto timestepper turned on. That's why the analysis error terminates when the timestep fails to converge

First I would suggest that you run these models without augmented Lagrangian turned on. Check the penetration and adjust the penalty to reduce penetration if necessary, writing out the variable "contact gap" to the plotfile. Once again, this result has units of length. The best you should hope to achieve with the penalty method is about 1/10th the thickness of your elements at the contact interface.

Get all of your mesh refinement cases running with the penalty method (no augmented Lagrangian), adjusting the penalty scale factor individually for every case so that the max gap is similar. At that point, if you want, you can turn on augmented Lagrangian. I suggest that you do not use "gaptol", just use "tol" to control the norm of the lagrange multipliers. I typically use a value of 0.05 or 0.1.

Best regards,

Jeff Weiss

[moon]

Dear Mister Weiss

Thank you very much for your answer.
To turn off augmented Lagrangian and adjusting the penalty scale factor will be my next approach.

Best regards,

Moon