Centrifugal Force Contact Problem

Dear all,

I try to simulate one quarter of the rotor of an electrical machine with centrifugal force loading. Therefore, I modeled the rotor with Gmsh and imported the mesh. The magnet (cuboid) inside the rotor isn’t tied with the other material (iron), so I want to model a contact. My problem is, that it looks like the contact is completely ignored. I already tried various things, sometimes I didn’t get convergence:

  • using node-to-surface contact
  • changing the contact factor (from 1e2 to 1e20)
  • using a 2D model
  • using a magnet with more thickness compared to the iron and vice versa
  • using only the surface above and under the magnet as contact surface

Interesting: It worked when I used a constant displacement of the magnet in radial direction (cylindrical coordinates) instead of the centrifugal force. So maybe it has something to do with the loading?

I attached a picture of the ignored contact and the files.

files: https://drive.google.com/file/d/1v1ilR3USqRlF2acm8Dpn3zHitYxla04M/view?usp=sharing (execute the .fbd file)

I would appreciate any help!

Best regards.

It seems that some of the include files are missing, making it impossible to run this analysis. Can you add them ?

1 Like

Hello Calc_em,

I can run it if I execute the .fbd file. I have added all files now: https://drive.google.com/file/d/1v1ilR3USqRlF2acm8Dpn3zHitYxla04M/view?usp=sharing

All right, I don’t use GraphiX so I was trying to submit it directly using ccx. But now it works with all the files.

When I look at the results with deformation scale factor set to 1 to see the true deformation, I can’t see any large penetration, there’s just some small movement and contact at the edges of the magnet.

Btw. prescribed displacement is usually much better than force load for analyses involving contact.

1 Like

It seems you try to model it as a 2D problem (I’d rather use plane strain elements than plane stress) but then the final mesh is 3D with linear tetras :thinking:…I’d try to perform it using 2D plane strain 4 node quadrilaterals, maybe refining the mesh. Nevertheless as Calc_em said you have little penetration so solution seems good, if you scale that penetration is normal nodes aren’t coincident to that scale

1 Like

@Calc_em You are completely right, apparently the rotation speed is too low (it should be Xe6 instead of Xe4). Then, I think it looks good:

Thank you for your input.

@JuanP74 I already tried a 2D model, but this isn’t so easy with the Gmsh import and I’ve got some convergence problems. At the moment, the 3D approach looks more promising. But I will try it later again.

1 Like

I got it to work using plane strain elements. Most interesting to me was that I have to use the following contact parameters that I evolved from this post (Convergence issue in 2D contact problem):

** --------- Contact ---------


link to files: Rotor_with_magnet_all_files - Google Drive

1 Like


I think the problem here is purely related to the behavior of the physical problem. Two parallel surfaces in contact to each other and rotating perpendicular to the radius & axis of rotation are at a point of unstable equilibrium. Any inclination/deviation however small of the magnet will cause it to fly away if not prevented by:

Lateral restraint

Once that is understood, the problem can be solved in multiple ways and even improve the design (I would give them a small curvature to increase the contact area if it does not compromise the performance of the machine).


1 Like

nice :ok_hand:, what contact parameters did you use in your analysis?