How to correctly simulate interference in MES?

[giorgio.ramorino]

Hello,

I have a question regarding MES Simulation.

I would like to know wich is the best way to simulate interference between parts with this kind of analysis.

I already am able to obtain the stress results in the static linear one, but I can't do the same in MES since there is no shrink fit contact.

Let's say I have a cilinder with a radius of 15 mm and a pipe with the internal radius of 14,9 mm.
I already have them in position in the assembly and with the interference. 

How do I obtain the stresses and strains due to the interference with MES?

Thanks

[John_Holtz]

Hi @giorgio.ramorino

1. I would start by creating a matched mesh. This will remove the interference from the CAD model. (I assume that you are using a CAD model.)
2. Then I would create surface contact between the two surfaces. 
3. Then I would define a User-defined contact distance equal to the amount of interference. (right-click on the contact pair in the browser and "Edit Settings > Advanced > Contact distance > User-defined"). This push the two surfaces apart until their separation is equal to the contact distance.

Although the same thing can be done with an unmatched mesh, the reason to create a matched mesh is to avoid the "interference" that occurs because the mesh only approximates the circular surfaces. See Figure 3 and the discussion on the page "Set Up and Perform the Analysis > Analysis-Specific Information > Nonlinear Analysis > Surface-to-Surface Contact > Surface Contact Settings > Simulation Mechanical Surface Contact Options (Nonlinear) > Advanced Tab" in the Help User's Guide.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[giorgio.ramorino]

Hello John,

thanks for your reply, I tried to do as you say but i still get the same problem. The contact is not simulated.

I noticed that even if i keep match mesh option the program doesn't eliminate the interference while meshing, you can see in the figure attached that i can see the 2 surfaces meshed at the interference distance, thus also the matching doesn't work well.

Do you know how could this happen? 

Thank you.

[John_Holtz]

Hi @giorgio.ramorino

You may need to set the contact type to "bonded" for the surface, generate the mesh, and then change the contact type back to "surface". The software probably "knows" that surfaces in contact in an MES analysis do not need to have a matched mesh.

Here is a little more information on what to look for in the mesh.

You are probably correct that the mesh is not meshed matched, but it is hard to tell from the image. It looks like you show the mesh on the outer part; you also need to look at the mesh on the inner part. If your image shows the surfaces of the CAD parts, those do not change. Because of the mesh matching (once you get it to work), the mesh on one of the parts will not follow the original CAD surface. I do not remember how the mesh matching works, but it probably moves the mesh on one of the parts to match the mesh on the other. I do not think that it will move the mesh on both parts to "split the difference". (You can use the "View > Appearance > CAD Surfaces" to show or hide the original CAD surfaces.)

[Royce_adsk]

Hi @giorgio.ramorino

Just checking in to hear if the comments from @John_Holtz allowed your to successfully move forward on your project?  It would be great to hear the current status of your analysis!

Cheers,

[giorgio.ramorino]

Hello,

sorry i still can't solve the problem.

I tried as you said but nothing, it just runs all the steps and give me a zero stress solution.

I also tried to import the steps with zero gap between the surfaces and then tried to give the interference using the user defined contact distance in the contact settings but it didn't work either.

[John_Holtz]

Hi @giorgio.ramorino

A result of 0 stress implies that there is no interference (or no contact). And the second situation implies that it didn't work. 

My suggestion is to create an archive of your model ("app button > Archive > Create") and attach the .ACH file. That way, we can look to see specifically how you have the model setup, what needs to be changed, and so on.

Alternatively, you can take a look at my model attached. It contains 4 design scenarios that are setup and ready to be analyzed:

1. linear static stress using shrink fit contact.
2. MES analysis using a matched mesh and surface contact distance equal to the interference
3. MES analysis using an unmatched mesh (interference left in the model) and surface contact distance = 0
4. MES analysis using temperature to heat (or shrink) one part to slowly create the interference. I did this method because the other methods cause the interference to be applied instantaneously. This can cause convergence problems in some models. (Of course, thermal expansion can cause other problems in the analysis if you are not careful, such as thermal stress.)

[giorgio.ramorino]

Hi John,

thanks for you time.

I looked your simulations and the one i would like to manage to replicate is the 3rd one.

For my final aim I cannot use mirror planes, and the interference is 0.1 mm on the radius,  but for the rest the situation is the same.

I tried to do for my parts what you did, but still i didn't get the results.

I attach here the .ach file so you can have a look at it if you are so kind.

I noticed that if i increase the dimension of the mesh it seems at least to notice the interference (but then the mesh is too coarse and it just does 2 steps and then no convergence)

[John_Holtz · Accepted solution]

Hi @giorgio.ramorino

Contact is not being detected in your setup because it has "too much penetration". There is some logic that if the parts penetrate "too much", it is probably not giving the results that you want. When that occurs, the analysis ignores the contact!

So the solution in your model to have the contact detected is to increase the allowable penetration.

The next problem is going to be that it is hard to converge when you immediately impose an interference fit. The parts want to vibrate and rotate and move to find an equilibrium. You might need to run the analysis with a lot of very small time steps to get it to converge and settle down, and then use larger time steps to apply the live loads.