I faced a issue when I try to simulate a dynamic motion between different connectors.
The structure shows as below picture.
However, the part isn't move at all.
No deformation or stress shows.
Could you tell me where I do wrong?
Sorry, but I didn't understand how to add [metal spring-form and the "plug"] to my simulation.
And I also took off the big flat board and using static structural.
And I tried to use translational joint in my simulation, but the the result still not correct.
The below picture shows how I do my simulation.
Where should I add spring-form?? and how to do it correctly??
Hello, I think Peter is just referring to the parts (the green one in your case). What are your parts named?
When you say that the results are incorrect, what do you mean and how?
The "spring form" I mean is the green one with the brown liner. How is the brown liner fastened to the green part? If it is fastened, you should have a bonded contact between the green and brown parts.
The "plug" is the grey part.
I see the grey plug has a sharp corner where it is touching the brown spring. That will create very high stress on that corner. I recommend adding a blend radius to that corner so you have face to face contact, not edge to face contact when the displacement starts pushing the parts together.
To do this insertion of the spring form over the fixed plug, you don't need so much geometry.
Suppress the light grey long part and move the Fixed Support to the back face of the plug where the light grey part used to be.
Make a cut through the green part, about a plug length back from the base of the brown part. Put a translation joint on that cut face so that it is free to move along the right direction.
Use a joint load to add a displacement to move the spring form over the plug.
If you create a Workbench project archive .wbpz file, you can attach it to your post.
The contact between green one and brown liner is "No Seperation".
However, I still don't understand how to make a cut through the green part.
Also, how to add a joint load?
Also, I already save my project as a .wbpz file, please refer to the attached file.
Model building and solving.
The next step is to do a Mesh Refinement Study and add more substeps to fill out the force-displacement curve.
That is a fantastic explanation, I am sure we all learned something. Kudos to you for going through such an effort to explain.
I followed the steps in the previous video, but I still faced an error which shows .
Could you show me how to fix it?
Your model is probably not properly constrained somewhere. Please refer to this discussion by Peter and check out if the suggestions listed here help?
Thanks for updating your username on this site. Much easier to say!
Here is my video response using your model.
I moved the parts 12.5 microns closer together, but I forgot to subtract that number from the Joint translation load. You should include editing the Joint translation to the steps shown in the video to avoid moving the parts too far.
I followed the steps in your video, but still get the error message like this.
Could you help me figure out why??
This video shows two mesh refinements guided by the NR Force Residual Plots. The sweep method on the other part that resulted in a failed mesh needs more investigation.
You can show your appreciation by clicking Like below the posts that are helpful.
I figured out why the other part had a failed mesh. The geometry has some inaccuracy that creates a tiny edge.
I tried the way you mesh, but still can't get the result.
Could you take a look of my simulation file?
The NR Residual Force plot tells you what it needs, smaller elements around this area.
Form New Part in DM, suppress the Bonded Contact. Use Virtual Topology to repair the small edges on that part.
Add a sweep on that part and set the number of divisions to 2 on the sweep.
Then the solver will be able to finish.
Thank you for your helpful hints and video.
I solved most of my simulations, but there is still a model I can't solve even I change the mesh and using virtual topology.
The simulation stock at some place shows in the below picture.
Could you show me how to correct my mesh to simulate this model?
Please see if these tutorials on Meshing help.
I tried many different way to generate the mesh.
But the workbench still shows the error message like this: The solver was unable to converge on a solution for the nonlinear problems.
And I don't know how to solve this issue.
Could you give me some hint?
I downloaded your archive and am running it now to find the point at which it fails.
I expect breaking up the displacement so that the range where it gets into trouble is a separate step so that very small substeps can be used may be one method.
Another method to help contact models make progress is to modify the Normal Stiffness.
Getting these models to converge is time-consuming (and frustrating) so the best advice I can offer is to slice the model twice, one plane at half the thickness and a second plane through the center so that only one half of one fork of the clamp is riding on one side of one half of the plug. Symmetry BCs keep the model working the way the full model does now, but the model solves four times faster!
I will report with an update, but get going on those two planes to cut your model down to a 1/4 model. The other time saver is the multibody part and eliminating the bonded contact, but that is a smaller benefit than the 1/4 symmetry.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.