How to simulate two connectors motion?

  • 361 Views
  • Last Post 25 September 2018
Han-yu posted this 06 August 2018

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 06 August 2018

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 06 August 2018

 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 06 August 2018

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 06 August 2018

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 07 August 2018

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 08 August 2018

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

 

SandeepMedikonda posted this 08 August 2018

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 11 August 2018

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 11 August 2018

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 12 August 2018

 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

peteroznewman posted this 12 August 2018

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 12 August 2018

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 12 August 2018

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

peteroznewman posted this 12 August 2018

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 12 August 2018

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 13 August 2018

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
Han-yu posted this 20 August 2018

Hi Peter:

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?

Thank you.

Attached Files

SandeepMedikonda posted this 20 August 2018

Han-yu,

  Please see if these tutorials on Meshing help.

Regards,

Sandeep

  • Liked by
  • Han-yu
Han-yu posted this 21 August 2018

Hi Sandeep:

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?

Thank you.

 

Best Regards

Han-yu

peteroznewman posted this 21 August 2018

Hi Han-yu,

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.

Regards,

Peter

  • Liked by
  • Han-yu
SandeepMedikonda posted this 21 August 2018

Han-yu,

  I am unable to open your model, so Peter might be able to help.

One thing I did notice from your picture is that you only had 2 elements in the through the thickness. So the aspect ratio for these elements must be quite bad? Is this due to the limitation in the number of elements of the student version?

Regards,

Sandeep

peteroznewman posted this 22 August 2018

Hi Han-yu,

I agree with Sandeep, that two elements though the thickness is too few. Below is the model after being sliced into a quarter model.

I saw the original model failed at a time of about 0.8, so in this quarter model.

I tweaked the Translate in DM to 25.9 microns because there was a significant gap and I wanted to turn off Adjust to Touch. Now the contact is closed at the start of the simulation.

I break the displacement into four steps. Step 1 has 0 displacement and is just to let the initial contact develop using 5 substeps. Step 2 used -0.0095 mm and I use minimum substeps of 200 to let the displacement get through the transition from the tip to the bump. Step 3 is the easy step along the length.  Then Step 4 has the final displacement to get through the difficult section to ease the clasp into the well.

I will see how well this strategy went in the morning.

Regards,

Peter

 

  • Liked by
  • SandeepMedikonda
  • Han-yu
peteroznewman posted this 22 August 2018

Hi Han-yu,

Step 2 had too short of a displacement, so it failed and I made it larger. I also wanted to cut the simulation time in half again. Look at the deformation in the clip. It is 16 micros in the X direction while the plug has only moved -0.07 microns in the X-direction.  This is good evidence that changing the plug to a rigid body will not incur a significant error in the clip stress.

That let me get to a complete solution after I replaced the Fixed Support with a Fixed Joint on Polyline13.

Here is the Force vs. Displacement chart for the 1/4 model, start to finish is right to left on this chart.  This chart has to be multiplied by 4 for the full model. 

Both the Stress and the Force are the result of a linear elastic material model. Since the stress has gone way, way past the yield and ultimate strength of the nickel and silicon materials, the Force result does not represent reality.  In order for this simulation to represent reality, plasticity should be added to the nickel material. I guess silicon does not behave with plastic deformation beyond yield, I guess it shows a brittle fracture at its ultimate tensile strength. I don't know what that value is, but it is time to start paying attention to it.

Here are the Analysis settings for this run.

Here is the joint displacement.

Here is the Frictional Contact details.

Here is the convergence plot. The steep part in the middle of the Time plot is the long stroke with the bump on the side which can take large substeps between the difficult start and end part of the stroke that required small substeps.

 

Let me know if you can get your model to run with these settings and mention the version of ANSYS you are using.

Regards,

Peter

  • Liked by
  • Han-yu
  • jonsys
Han-yu posted this 24 August 2018

Hi Peter:

Thank you for your hint and solutions.

I was able to run the simulation.

But I applied the some solution on another simulation, it doesn't work.

Is these solutions can only be applied to certain simulation?

Or the attached simulation is special?

Thank you.

 

Best Regards.

Han-Yu  

Attached Files

peteroznewman posted this 25 August 2018

Hi Han-yu,

Change Sweep Method 2 > Sweep Num Divs from 2 to 4 and it will start converging.

Best regards,

Peter

  • Liked by
  • Han-yu
Han-yu posted this 27 August 2018

Hi Peter:

May I ask how do you know the Sweep Method 2 needed to be changed?

Based on experience? or there is some other rule need to follow while I creating the mesh?

Thank you.

peteroznewman posted this 27 August 2018

Hi Han-yu,

When the solution fails to converge, you look at the Newton-Raphson Force Residual Plot and it shows you the problem is on the elements created by the Sweep Method 2.  They also have the worst aspect ratio and the fewest number of nodes along the sweep. Those are all the clues that said to try 4 instead of 2 elements.

Regards,

Peter

  • Liked by
  • Han-yu
  • jonsys
Han-yu posted this 27 August 2018

Hi Peter:

I follow your instruction and try to solve it last night.

But the simulation still failed.

Is there any change you make beside change the sweep method 2?

Thank you.

Attached Files

peteroznewman posted this 27 August 2018

The unmodified model with 2 elements wouldn't start converging on step 1. The only change I made was to make it 4 elements then it did start converging through step 1. That modified model did not make it all the way. It failed to converge here:

But in this case, the reason it stopped is because the displacement was larger than needed and the part ran into the other wall.

I have attached the ANSYS 19.1 archive that I solved.

Attached Files

  • Liked by
  • jonsys
Han-yu posted this 27 August 2018

Hi Peter:

There is another question we interested in which is the contact force and contact area in this model.

I tried to figure out this question with the "Probe"-> Force Reaction.

But the setting seems wrong.

Could you kindly tell me where I do wrong?

Thank you.

Show More Posts
Close