Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
hyperelastic material in contact with a rigid material
Posted 11 mar 2013, 12:36 GMT-4 Structural Mechanics 4 Replies
Please login with a confirmed email address before reporting spam
I'm trying to model the stresses in a hyperelastic material as it's removed from a highly rigid material (which is acting as a mold). I've set up a time-dependent model with the two materials, a contact pair with friction between them, and prescribed a velocity at the top of the hyperelastic material, but am having convergence problems.
I've tried playing with the meshing (mapped works best), the material properties, the initial values (mod1.u should be initial-value based) and several other things. For the lowest-strain cases (the first value in the parametric sweep in the attached file) the simulation runs fine, but for the higher-strain cases (all other values), the simulation fails before completion.
I'd appreciate any suggestions you have as to how I could improve this!
Kind regards,
Allison
I've tried playing with the meshing (mapped works best), the material properties, the initial values (mod1.u should be initial-value based) and several other things. For the lowest-strain cases (the first value in the parametric sweep in the attached file) the simulation runs fine, but for the higher-strain cases (all other values), the simulation fails before completion.
I'd appreciate any suggestions you have as to how I could improve this!
Kind regards,
Allison
Attachments:
4 Replies Last Post 12 mar 2013, 15:27 GMT-4
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Allison,
Without taking a detailed look at your model, my first suggestion would be to try to solve this problem without the hyperelastic material model first. Just use a linear elastic model for both domains. Then, make sure you can solve the contact problem for all parameters. Convergence issues are common in both contact modeling and especially in hyperelastic material modeling. I'd recommend first debugging the contact problem. Then add the hyperelastic complexity. If the problem is the hyperelastic material model, you can try playing with the parameters to decrease the nonlinearity of the model slightly and see if that helps.
Regards,
Josh Thomas
AltaSim Technologies
Without taking a detailed look at your model, my first suggestion would be to try to solve this problem without the hyperelastic material model first. Just use a linear elastic model for both domains. Then, make sure you can solve the contact problem for all parameters. Convergence issues are common in both contact modeling and especially in hyperelastic material modeling. I'd recommend first debugging the contact problem. Then add the hyperelastic complexity. If the problem is the hyperelastic material model, you can try playing with the parameters to decrease the nonlinearity of the model slightly and see if that helps.
Regards,
Josh Thomas
AltaSim Technologies
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Josh,
Thanks for the reply, and the suggestion. Unfortunately, I've already tried the same model with a linear elastic material and it doesn't make a significant difference. I'll keep digging!
Regards,
Allison
Thanks for the reply, and the suggestion. Unfortunately, I've already tried the same model with a linear elastic material and it doesn't make a significant difference. I'll keep digging!
Regards,
Allison
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Allison-
If the model isn't converging with a linear elastic material model, then you know there is a convergence issue probably with the contact modeling. I would work to troubleshoot and obtain convergence for the contact problem first using the linear elastic material model.
Here are some things to try to help with contact convergence:
1) Try using linear shape functions for displacement discretization. The default is quadratic.
2) Run the problem without friction before adding friction. Then, if friction causes the convergence issue you can adjust friction parameters.
3) Check that you are using the Double dogleg solver -- this should be the default in v4.3a but I'd check anyway. I've had good success with this new solver for contact problems.
4) Try making a good guess of the initial value of contact pressure.
5) Stiffer part should be the source.
6) There should be a finer mesh on the destination.
Best regards,
Josh
If the model isn't converging with a linear elastic material model, then you know there is a convergence issue probably with the contact modeling. I would work to troubleshoot and obtain convergence for the contact problem first using the linear elastic material model.
Here are some things to try to help with contact convergence:
1) Try using linear shape functions for displacement discretization. The default is quadratic.
2) Run the problem without friction before adding friction. Then, if friction causes the convergence issue you can adjust friction parameters.
3) Check that you are using the Double dogleg solver -- this should be the default in v4.3a but I'd check anyway. I've had good success with this new solver for contact problems.
4) Try making a good guess of the initial value of contact pressure.
5) Stiffer part should be the source.
6) There should be a finer mesh on the destination.
Best regards,
Josh
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
There are some issues in your model:
1, The internal core is almost rigid (E=1E8 GPa). No need to solve for it. Make it completely rigid instead by adding a Fixed constraint to the domain and remove the constraints form the boundaries.
2. The problem is not truly time dependent. The time is only used as a parameter. Replace the Time dependent study with a Stationary study, in which you use the Continuation solver (under Study extensions). Replace the prescribed velocity with Prescribed displacement having the value controlled by the continuation parameter.
3. Put a finer mesh at least in the axial direction of the hyperelastic part.
4. The scaling values of the Dependent variables for contact pressure and friction force are about four orders of magnitude too large. The effect is that you essentially have no convergence check at all on these variables.
Regards,
Henrik
There are some issues in your model:
1, The internal core is almost rigid (E=1E8 GPa). No need to solve for it. Make it completely rigid instead by adding a Fixed constraint to the domain and remove the constraints form the boundaries.
2. The problem is not truly time dependent. The time is only used as a parameter. Replace the Time dependent study with a Stationary study, in which you use the Continuation solver (under Study extensions). Replace the prescribed velocity with Prescribed displacement having the value controlled by the continuation parameter.
3. Put a finer mesh at least in the axial direction of the hyperelastic part.
4. The scaling values of the Dependent variables for contact pressure and friction force are about four orders of magnitude too large. The effect is that you essentially have no convergence check at all on these variables.
Regards,
Henrik