Cancel
Showing results for 
Search instead for 
Did you mean: 

Contact Pressure is not at expected contact point

Experimenter
Experimenter

Hello,

 

I'm trying to simulate the contact pressure and stress of a railway wheel on a rail. It's just a static analysis, so I've just been using SOL101. I do move the position of the wheel perpendicular to the direction of the rail so that I can see the different contact points on the wheel.

 

But sometimes I get solutions that look like this :

 

weird contact.JPG

 

 

Which doesn't look quite right. What exactly is happening and what can I do to avoid it?

 

I've set a surface to surface contact between the tread of the wheel and the rail. The .assyfem file refers to an assembly file in which I have also set a contact constraint between the wheel and the rail. Could this be the issue? I've looked at the contact area and it does look like there might be a bit of an overlap between the models, but I don't know what I can use to verify it.

 

Thank you.

7 REPLIES

Re: Contact Pressure is not at expected contact point

Creator
Creator

Could you share your files to check it?

 

Re: Contact Pressure is not at expected contact point

Change initial penetration in case control and check whether it helps.

Re: Contact Pressure is not at expected contact point

Experimenter
Experimenter

I've tried that and it doesn't do much. I've sort of fixed it by doing all the constraints again, but that means I don't quite understand what went wrong.

Re: Contact Pressure is not at expected contact point

Experimenter
Experimenter

Here are the files. It's not the same file as the one I initially showed, but it exhibits the same problem.

Re: Contact Pressure is not at expected contact point

maybe it is due to symmetry BCs. Does full model work ?

Re: Contact Pressure is not at expected contact point

Experimenter
Experimenter

Hmm. I will try that out. I have managed to get results that make sense before using symmetry, but I've been trying to get results where the wheel is moved so the contact point is at different points on the wheel tread surface. At certain lateral displacements I get problems with the contact results.

Re: Contact Pressure is not at expected contact point

Siemens Phenom Siemens Phenom
Siemens Phenom

I see several questionable items in the model that was posted:

 

  1. The presence of 2D shell elements in the analysis. I assume that these were the seed faces for a extrude/revolve mesh. I toggled off the "Export Mesh to Solver" setting on the Mesh Associated Data for these two meshes so that they would not be part of the analysis
  2. User defined constraint was applied to faces that were target faces of the RBE2 connection recipe. AUTOMPC really shouldn't be used to eliminate almost every dependent RBE2 DOF. The constraint should simply be applied to the same grid that the force is applied to and let the RBE2 handle the rest.
  3. INIPENE was set to 3. This eliminates both inital penetration AND initial gaps. Since this is a wheel on a rail, you don't want to artificially eliminate the initial gaps. This greatly expands the contact area (which theoretically should be point contact) and is the biggest source of error in this problem.

The attached updated model addresses all of these issues. Contact pressures look as expected (nearly point contact on both the wheel and the rail.

 

ContactPressure_Rail.pngContactPressure_Wheel.png