How to simulate two connectors motion?

  • 105 Views
  • Last Post 2 days ago
Han-yu posted this 2 weeks ago

Hi:

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?

 

 

 

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

What is wrong

  • Using a non-zero Displacement in Explicit Dynamics.
  • Using Explicit Dynamics.

What to do instead

  • Do this model in Static Structural first.
  • Move the parts closer so the metal spring form is tangent to the first surface it touches when the contact begins.
  • You don't need the big flat board to control the axial motion of one part, use a translational joint.
  • I gave you some good suggestions here.

Han-yu posted this 2 weeks ago

 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??

Thank you.

SandeepMedikonda posted this 2 weeks ago

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?

~Sandeep

peteroznewman posted this 2 weeks ago

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.

Regards,
Peter

 

 

Han-yu posted this 2 weeks ago

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.

Thank you.

Attached Files

peteroznewman posted this 1 weeks ago

Hello Virginia,

Model building and solving.

 

Results

 

The next step is to do a Mesh Refinement Study and add more substeps to fill out the force-displacement curve.

Regards,
Peter

 

  • Liked by
  • SandeepMedikonda
  • Han-yu
SandeepMedikonda posted this 1 weeks ago

Hello Peter, 

That is a fantastic explanation, I am sure we all learned something. Kudos to you for going through such an effort to explain.

Regards,

Sandeep

Han-yu posted this 4 days ago

Hi

I followed the steps in the previous video, but I still faced an error which shows .

Could you show me how to fix it?

Thank you.

 

 

Attached Files

SandeepMedikonda posted this 3 days ago

Hi

Your model is probably not properly constrained somewhere. Please refer to this discussion by Peter and check out if the suggestions listed here help?

Regards,

Sandeep

peteroznewman posted this 3 days ago

 Hi Han-yu,

Thanks for updating your username on this site. Much easier to say!

Here is my video response using your model.

 

Regards,

Peter

  • Liked by
  • SandeepMedikonda
  • Han-yu
peteroznewman posted this 3 days ago

Han-yu,

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.

Regards,

Peter

  • Liked by
  • Han-yu
Han-yu posted this 3 days ago

Hi

I followed the steps in your video, but still get the error message like this.

Could you help me figure out why??

Thank you

Attached Files

peteroznewman posted this 2 days ago

Hi Han-yu,

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.

Regards,
Peter

  • Liked by
  • Han-yu
peteroznewman posted this 2 days ago

Hi Han-yu,

I figured out why the other part had a failed mesh. The geometry has some inaccuracy that creates a tiny edge.

 

Regards,
Peter

  • Liked by
  • Han-yu
Han-yu posted this 2 days ago

Hi Peter:

I tried the way you mesh, but still can't get the result.

Could you take a look of my simulation file?

Thank you.

Attached Files

peteroznewman posted this 2 days ago

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.

 

You can show your appreciation by clicking Like below the posts that are helpful.

Regards,

Peter

 

  • Liked by
  • Han-yu
Close