## General Mechanical

#### How to simulate two connectors motion?

• Han-yu
Subscriber

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?

• peteroznewman
Subscriber

### 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
Subscriber

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.

• Sandeep Medikonda
Ansys Employee

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
Subscriber

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
Subscriber

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.

• peteroznewman
Subscriber

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

• Sandeep Medikonda
Ansys Employee

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
Subscriber

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.

• Sandeep Medikonda
Ansys Employee

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
Subscriber

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
Subscriber

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

• Han-yu
Subscriber

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

• peteroznewman
Subscriber

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
Subscriber

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

• Han-yu
Subscriber

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.

• peteroznewman
Subscriber

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

• Han-yu
Subscriber

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.

• Sandeep Medikonda
Ansys Employee

Han-yu,

Please see if these tutorials on Meshing help.

Regards,

Sandeep

• Han-yu
Subscriber

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
Subscriber

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

• Sandeep Medikonda
Ansys Employee

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
Subscriber

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

• peteroznewman
Subscriber

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

• Han-yu
Subscriber

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

• peteroznewman
Subscriber

Hi Han-yu,

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

Best regards,

Peter

• Han-yu
Subscriber

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
Subscriber

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

• Han-yu
Subscriber

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.

• peteroznewman
Subscriber

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.

• Han-yu
Subscriber

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.

• peteroznewman
Subscriber

Hi Han-yu,

1. If you want the insertion force data, add a Probe for Joint Load Reaction Force.

2. If you want the contact pressure, you can get that by inserting a Contact Tool in the Solution branch and insert Pressure.

3. Finally, there are some contact items that are not written to the output results unless you request them. You do that here:

then you have to solve again!  But you probably wanted item 1 or 2 above anyway.

Regards,

Peter

• Han-yu
Subscriber

Hi Peter:

I tried your solution to change Mesh sweep way from 2 division to 4, 6,8 division.

But the simulation still not working.

Is it because my Ansys version is not the newest? My workbench version is 16.0.

Is there another solution I can apply?

Thank you.

• peteroznewman
Subscriber

Hi Han-yu,

It could be that 19.1 can solve it as is, but 16.0 can't without more help.  I have version 16.2 still installed on this computer.  Archive your model, attach it to your post above and I will try running your model under 16.2 to see what has to change to get it running. I doubt there is much difference between 16.0 and 16.2.

I suggested you use a Rigid behavior on the Nickel body on the plug, since there is almost no deformation on that side. That would cut the number of elements that have to converge in half.  That might help.

I suggested you use symmetry on two planes to cut the model in half again and again. That will cut the number of elements that have to converge to a small number. That might help.

Regards,

Peter

• Han-yu
Subscriber

Hi Peter:

I attach my model to the previous post.

Please refer it and help me run it on Ansys 16.2.

Thank you.

• peteroznewman
Subscriber

Hi Han-yu,

The only change I made was to take a zero out of the element size in this Face Sizing mesh control.

Now it is converging in ANSYS 16.2

Regards,

Peter

• peteroznewman
Subscriber

You still are pushing the joint too far.  Below is the Joint Probe of the Force to translate the Joint.

You can see that step 3 could have been a little longer before the small substeps of step 4 begin.

• Han-yu
Subscriber

Hi Peter:

Sorry to bother you again.

I faced a nonlinear converge problem, and the mesh size is limited by the current license.

The error messages are show below.

Could you help me take a look of my simulation?

Thank you.

• peteroznewman
Subscriber

Hello Han-yu,    [Edited]

I'm glad to see you using Symmetry, but you didn't add in a Displacement BC to support the symmetry plane. Please add X=0 to the four faces.

You forgot to suppress the automatically generated Contact 7 that is bonding your sliding interface.
In Workbench menu use Tools > Options and uncheck the Auto Detect Contact On Attach and you will never have to worry about that again!

I took a 0 out of your Face Sizing to reduce the mesh density since a lower density ran well in an earlier model.

I added a Command Snippet to the Static Structural branch that has the code:

NEQIT,60

which forces the solver to keep trying for longer than the default 26 iterations.

In Step 1, I turned off Auto Time Stepping and set the Substeps to 1.
I also made Step 2 have 500 Initial and 500 Minimum Substeps.

In DM, I added a plane at the center of the thickness and created another plane of symmetry. This cuts the aspect ratio of the elements in half and provides the second plane that removes the need for a translation joint.

I removed the translation joint and replaced it with a displacement on that same face.

I made sure I was solving in the units of microns.

You can make those changes now and see if your model converges.

Regards,

Peter

• Han-yu
Subscriber

Hi Peter:

I suppressed the bond contact, so the simulation can go longer.

But it still stuck as below picture shows.

Could you teach me where should I modify?

Btw, how could I add Command Snippet to this simulation?

And the X=0 to four faces?

Thank you.

• peteroznewman
Subscriber

Hello Han-yu,

All the changes are incorporated in this archive that seems to make good progress. The X=0 Displacement is only on two faces of the flexible body. It doesn't apply to the Rigid body.

The only change I would make is to the Minimum Substeps in Step 2. 500 is larger than necessary. Back off to 100.

The ANSYS 16.2 archive is attached.

Regards,

Peter

• peteroznewman
Subscriber

Model stopped shortly into Step 3. Here is the Force-Displacement curve for pushing one-quarter of a clip into the plug. Multiple this value by 4 to get the full model reaction force.

The force that is shown above is not real, it is an artifact of using linear elastic materials in a model that takes them past their point of failure. Therefore if the clip would have broken.

The maximum tensile strength of Pure Nickel that I found was 1000 MPa, which has been colored red below, and the yield strength was 935 MPa. Annealed Nickel had much lower values.  It is difficult to find the ultimate tensile strength for silicon, but one reference was 120 MPa.

If your goal is that this clip does not break off, then you are bending it too much and you should consider a design change.

Regards,

Peter

• jackhero
Subscriber

@Peter,

Thank you for the detail video for solving the model and useful information regarding the convergence problems. With reference to your video post link here, I would like to ask how did you estimate that the solution has passed the 10% or 20% or 30% point? To be precise you mentioned about it around time 9:00 minutes of above mentioned video.

• peteroznewman
Subscriber

Jack,

When the solution has a time step of 1 and the time is at 0.3, that is 30% of the way through the solution.

This Discussion is too long, so when you have a question on an old discussion, just create a New Discussion to ask your question and you can put a link into the old discussion for reference.

Regards,

Peter

• kaitova
Subscriber
Hi dear Peter,,I am trying to run simulation that you were so kind to describe here and explain to the user. I am trying to rerun it myself. Would it be possible for you to check my mistakes as I can not succeed in this simulation. Thank you in advancen