ERROE"Negative jaction was detected"

[david194]

Hello,
I am a medical student and I am new to FEbio. I am trying to run a dynamic hip model with biphasic material cartilage. I am focusing on contant stress and fluid pressure. The load is gait data and the force has two peaks at time1.2 and 1.6 respectively. First I tried to use simple material parameters and the model converged some of the time, but when I doubled elements of the acetabular cartilage it did not converge. On the other hand, I tried complex material parameters, and the model always failed to converge beyond time1.5, even though I had refined the mesh.
I have read FEbio User Manual and Studio Manual, tried both the penalty method and the augmented Lagrangian method, and adjusted Time Stepping, but there is no significant improvement.
Please give me some suggestions on how to adjust the parameters to converge the model.
Thanks,
David

[ateshian]

Hi David,

I couldn't download your model without having to sign in on Google Drive. Can you please share it using a method that doesn't require logging in?

Best,

Gerard

[david194]

Hi Gerard,
I have changed the download link, please try again.https://drive.google.com/drive/folde...Pu?usp=sharing
Thanks,
David

[ateshian]

Hi David,

I suggest you try the following:

1) In the sliding-biphasic contact interface turn off "update penalty". Since you are using the AUGLAG setting, this should not compromise your analysis but may improve convergence. As the hip contact force increases, the contact gap in your analysis is similarly increasing to large values (approaching 0.8 mm). So set the tolerance for the AUGLAG scheme to 0 and set the gap tolerance to 0.1 mm. This may increase the number of iterations at each time point, so you should increase the opt_iter parameter to 25.
2) For the first Step (contact), reduce the number of time steps from 10 to 1 and increase the step size (and max step size) from 0.1 to 1.0. This step converges easily, so there is no need to waste time with multiple time steps.
3) For the second Step (gait), increase the number of time steps from 10 to 50 and decrease the step size (and max step size) from 0.1 to 0.02. This will take longer to run, but you will capture the full gait response more faithfully.
4) To run the model faster I suggest switching the linear_solver to Mkl_dss (for both steps).
5) To make sure that the analysis remains valid at each time step, set dtol=0.001 and ptol = 0.01 (you had changed them to 0).

Please try these things on your simple model first. If satisfied, move on to the complex model. With these settings I was able to run your model to completion.

Best,

Gerard

[david194]

Hi Gerard,
Thank you so much for your suggestions, they really helped me.
One thing I noticed was that the results fluctuated around 1.6 second while the curve was relatively smooth at other times. I checked the contact surface of the acetabular cartilage model and there was some unusual deformation of the surface elements (I'm not sure how to describe this state). Does this mean that the quality of elements is not good enough, or is there something else wrong?
Thanks,
David.

[ateshian]

Hi David,

This phenomenon is called the "hourglass effect", you can look it up online. In general it occurs when the mesh is unable to satisfy all the constraints of the governing equations. Perhaps you can try reducing Poisson's ratio for the deep zone elements from 0.4 to a smaller value (in biphasic analyses with fiber-reinforcement, it would be okay to set Poisson's ratio of the ground matrix to zero, with no harm -- that might eliminate this hourglass effect).

Best,

Gerard

[david194]

Hello Gerard,
Thanks for your answer.
I applied only one Z-axis force in the previous model and it worked after following your advice. When I added X and Y axes of force, it again became difficult to converge, even though I removed the rotational motion of the femur.I'm wondering what role do values of dtol and ptol play in the analysis and when can I set them to 0? On the other hand, are there any parameters that need to be changed?
Best regards,
David.

https://drive.google.com/file/d/1jYuZGfwKFTm8KuiC5AP93hYzPHHp-WJ2/view?usp=sharing

[ateshian]

Hi David,

FEBio solves nonlinearly for nodal deformations and fluid pressures using an iterative scheme. dtol and ptol represent the relative tolerances for determining if the nonlinear solution at a given time step has converged. If you set them to zero, you are asking FEBio to not use these criteria for detecting convergence, and that usually degrades the quality of the numerical solution. Using looser convergence tolerances might produce faster convergence for a few time steps, but as the solution becomes progressively less valid you may find that your model may no longer run to completion. So I recommend keeping the default values for dtol and ptol to avoid this problem, even if this means that the solution takes longer to converge.

Best,

Gerard

[david194]

Hello Gerard,
Thank you for your explanation, I will try more with reference to your comments.
Best regards,
David.