Frictionless support to run a 1/8 symmetry problem

Hi folks!

I’m trying to solve a problem that is a disc under centrifugal loading. I know that it is possible to simplify the geometry in a 1/4 model using the displacement boundary condition to impose the axisymmetry on PrePoMax. Nonetheless, in the case I’m working on, it is possible to simplify to a 1/8 model. Is it possible to set a frictionless support to constrain DOF only in normal directions on an edge? My intention is to set the “frictionless supports” constraining de DOF in edge normal directions like in the figure below:

Sem título

In CalculiX, there’s a cyclic symmetry feature for that. Not yet supported in PrePoMax but you can add it using keywords: Cyclic symmetry

1 Like

Thank you @FEAnalyst! I hadn’t seen your post. It will help me a lot!

I agree with you. It would be very useful to have this functionality in GUI.

1 Like

Another approach could also be to use a new coordinate system and define the supports based on it. But cyclic symetry is probably the better choice.

That’s right, the *TRANSFORM keyword can also help in this case.

1 Like

It is a nice suggestion. I’m going to test both options! Thank you.

Hey guys, it worked. Thank you all!

1 Like

Are those offsets, right?

I mean, you first requested for a frictionless support. There shouldn’t be any misalignment between undeformed and deformed model at the boundary ¿isn’t it?


1 Like

The 3 web spots holding the magnets are so very thin. Careful with that. I guess that’s why we do FEA right? lol.

1 Like

This is actually what I’m looking for now. I had this same misalignment between undeformed and deformed models in Ansys Mechanical. I’m studying the equations behind this symmetry condition technique to understand why it happens. I had used in the past only frictionless support to constraint DOF in edge normal directions to impose the symmetry condition.

It is a case where the body is under centrifugal acceleration. This load is added to the model by “centrifugal load”. Probably, this misalignment came from an approximation to solve the rotation as a static load.

Your deformation is not symmetric, because of the very thin details with only one element over the thickness. You have bending in that area and with only one element it is difficult to calculate the same deformation. You need a mirrored mesh to get a absolute symmetric result.

I made in Ansys Mechanical a 10th part model of a wheel. Mirrored the mesh and then rotated the mesh 5 times to get the same symmetric damage result on every spoke.

More information about the wheel model

Is it also possible to mirror the mesh and merge the nodes in PrePoMax?

1 Like

Is it possible that the model is under constrained (rigid body rotation) ?

I don’t know if building a mirrored mesh in PrePoMax is possible. Although, I’m going to refine the mesh in thin regions. Thank you for the suggestions.

Yes, it is. I think that this offset is a rigid body displacement. The strains and stress are symmetric.

If you expect a mirrored result output field and to capture it, you need a mirrored mesh, why not split the model again and use only 1/2 of the current model?

No, that is currently not possible.

1 Like

Thank you for the suggestion. I’m going to try it.