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?
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.
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.
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?
Change Sweep Method 2 > Sweep Num Divs from 2 to 4 and it will start converging.
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?
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.
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?
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.
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?
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.
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?
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.
I attach my model to the previous post.
Please refer it and help me run it on Ansys 16.2.
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
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.
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?
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:
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.
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?
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.
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.