Contact type and tolerances

[Pablo2120]

Hi everyone,

I've troubles trying to simulate a contact problem between 2 pins and a plate. The plate has a first hole of 55mm diameter, and the first pin is also 55mm in diameter, but the tolerance (gap) between them is 0.01mm (Tolerance H7/g6). I drew, both (first pin and first hole) at the same diameter using Inventor. First question: ¿How can specify the tolerance in Simulation Mechanical and what kind of contact should I use in that case?. Ok, that's the first problem.

Second one. In the same plate I've a second hole of 38,5mm diameter and a second pin of 38mm diameter. That's because I don't want the second pin to hold the applied load, just prevent that the plate rotates due to a small torque that is generated.
Second question: ¿What kind of contact should I use between second pin and hole?.

I used modified NR with line search as a solver scheme. 10 time steps and Load curve as soft as I can.

I attached the .fem file and some photos (hope you could help me to set the correct parameters).

I would appreciate your help a lot. I've spent hours trying to solve it. Thanks! 

[John_Holtz]

Hi @Pablo2120,

Can you explain why the gap between the pins and part is critical? In other words, what will the difference be between an analysis that includes the gap and an analysis that assumes the gap is 0?

Another question: is there reason (other than the gap between the pins) to be using MES or a nonlinear analysis? (Sorry, but I did not have time to look at the model, which may have answered this question.)

The reason that I ask those two questions is that a linear analysis is much easier to analyze. Unless there is something nonlinear occurring (such as large displacement or nonlinear materials), I think a linear analysis will give acceptable results.

[Pablo2120]

Hi, @John_Holtz.

Ok. I'll try to answer you as best as I can (English is not my native language).

It's an interesting problem, which apparently is simple, but it is not.

We have a plate with 2 pins, but only one pin (the largest) must support the main load. Therefore, the largest pin was assigned a tolerance of 0.01mm (type H7 / g6, but left at 0mm for the simulation), and the second pin, the smallest, was assigned a tolerance of 0.5mm of diameter (0.25mm radius, that was drawn in the CAD). The purpose of the small pin is to only prevent the plate from rotating due to the action of the applied forces (note that the line of action of the applied forces passes under both pins, which generates a torque), but this second pin MUST NOT support the main load.

Note that if both pins had the same fit, the smaller pin would take up much of the load applied, perhaps half, which should not happen for some reasons of the rest of the design.

So, I thought about using a MES type analysis (since the plate will rotate a small amount), but I'm not sure that the parameters I entered are appropriate. I thought of doing a linear simulation with both pins adjusted to 0mm, analyzing the displacement obtained when applying the force, and then for the MES analysis to use said displacement, and thus avoiding the numerical instability.

I hope I have made myself understood correctly.

[John_Holtz]

Hi @Pablo2120

Your English is very good, so no need to worry about your reply. I understand your model better. Let me apologize for not responding sooner.

For future reference, the .FEM file is not the complete model. The best way to send a model (or store it for yourself) is to create an archive: "app button > Archive > Create".

But the .FEM file that you provided had enough details to be able to provide some ideas. One difficulty that may be occurring is that the mesh on the pins and matching holes are different sizes. So even though the CAD model may have had a gap between the small pin and its hole, the mesh looks like it is interfering. (This is described in more detail in Figure 3 on the page Advanced Tab in the documentation.) The ways to prevent any interference and preserve the initial gap are these types of things:

• Use a finer mesh to get a better approximation of the round pin and hole.
• Adjust the CAD model, using the information on the Advanced Tab page, so that the actual clearance in the meshed is more like desired.
• Alternatively, you can mesh the model so that the pin and hole have 0 clearance: this will align or match the meshes. Then manually change the mesh to make the desired gap. ("Draw > Pattern > Scale or Copy" to scale the diameter about the axis centerline.)

Here is how I would perform the analysis, at least to get started and provide some information about what happens:

1. Perform a linear static stress analysis.
2. Use surface contact between the large pin and the hole.
3. Assume the rotation to make contact with the small pin is insignificant, and therefore, suppress the small pin. Apply constraints on the bottom of the hole to prevent rotation of the model (Ty constraint)
4. When I did this, I got the results shown in the attached images.

The next analysis might be a linear analysis with the small pin included. To include the gap in a linear analysis, I would match the mesh between the pin and hole, then reduce the pin size, and manually create the 0.5 mm long gap elements (or 0.25 mm if the gap is the difference in the diameter) between the pin and hole, and run the analysis.

If there is something in the linear results that indicate a nonlinear analysis would be beneficial, the final analysis would be an MES.

Let us know if you have any questions. Feel free to attach an archive of the model if you have problems so that we have the complete input.

[Pablo2120]

Hi @John_Holtz,

I've solved this problem. Now I've no time to explain what have I done, but please, don't delete this post. I going to explain it in this week (Friday or Saturday), because it's a very interesting problem.

Thank you very much for your help. Give me some time.