Cyclic symmetry in assembly with contact.

[Anonymous]

Hi,
I defined my cyclic symmetry for the model below, but i encountered a problem. Part 1 moves in negative Z direction pushing outwards part 2 in a plus X direction - the problems is that part 2 is fixed somehow in the radial direction and cannot expand. Does the cyclic symmetry works in the assemblies with contact, has anyone encountered such problem ?  Thx ! 
P.S. Why the part is not totally covered with a mesh ? Despite this I got analyses converged, but results as mentioned above don't reflect reality. 

[John_Holtz]

Hi @Anonymous

Just to be clear, you are not using cyclic symmetry. In-CAD does not have that capability, so I am certain you are not using it . (Cyclic symmetry is when the displacements repeat from one face to another, such as this example from Simulation Mechanical. What you are doing is better described as symmetry in a cylindrical coordinate system.)

Your model opened differently on my computer. When I open it, the model is a 90 degree section of the full model instead of a 1/16 (?) model shown in your image. The model also warned that there were updates to the assembly or components that had not been applied. Perhaps those updates are related to the mesh issue that you mentioned.

The problem with your setup is the "Constraint 2" applied as a hoop symmetry constraint on the two faces of "v11_collet_90_025:1" (near the number 2 in your image). Those faces are saw cuts in real life. They should not have any constraints on them because the face is free to move in all directions at that location. By adding constraints to those faces, you are telling the software that the part cannot move radially without generating strain in the hoop direction. That is not what happens in real life. The hoop symmetry constraints are only needed on the small face at the inner radius.

[Anonymous]

Hello @John_Holtz,

Thank you for the clarification, I will remember this now 🙂

I upload the model once again. What i noticed is that model is fully meshed when the cylindrical system is created for the outer diameter of the part number 2.

I constrained the model exactly as here, where we discussed it - maybe I misunderstood something. 
https://forums.autodesk.com/t5/nastran-in-cad-forum/another-interference-fit-analysis/m-p/8212421#M4...

When I am applying constrain as described by you, cannot get anything even close the reality - - maybe I am missing something.  Thx John.

[John_Holtz · Accepted solution]

Hi @Anonymous,

It took a while to sort out all of the issues, but I think that it works now. (Of course, my constraints may not be 100% correct because I am not that familiar with your model and the intent.)

The original discussion was for a complete cylinder with no slices (Figure 1), so symmetry constraints would be used regardless of where the full model is cut to create a symmetry model.

Figure 1: Model in original post

I do not know how to describe the new model (Figure 2), but I would say it is a cylinder but with 12 slices or saw cuts through 98% of the length. If you make a symmetry plane through the middle of a saw cut, you do not put symmetry constraints on the saw cut face; you only put symmetry constraints on the 2% of the length that is sliced by the symmetry plane. In the first model attached to this thread, you had the symmetry constraints applied to the full length, and that was the mistake.

Figure 2: Model in this post

In your second model attached to this post, you are holding small end of the locking sleeve in the axial direction, and trying to move it on the two side faces. Naturally, it will not move very well if you pull at one location and hold it at another! You need to put the axial constraints (Z direction in the local coordinate system) on the same faces where you have the enforced motion. (The enforced motions move the constraints, and the constraints move the model.) You may need hoop symmetry constraints on the two sides of the locking sleeve also. (I assume the locking sleeve is a full ring without any saw cuts.)

The next problem is that you need to specify a maximum activation distance for the separation contact. Since you are trying to move the locking ring 10 mm, you need to create enough contact elements to cover that distance, plus a little extra to extend to the next node. So a maximum activation distance of 15 is about right.

The last problem is with the mesh. For some reason, it passes through the body. That is why the mesh is not visible in some locations. (If you look at the results, you will see that the mesh on the collet is incorrect.) I corrected this problem by rebuilding and updating the mass in Inventor. ("Manage > Update > Rebuild All" and "Update Mass")

With those changes (and I think I changed a few nonlinear setup input), the analysis runs. See the attached file "2S_90_025 model 02.iam.zip". (I tried 3 variations: with and without friction, and with and without nonlinear materials. I was not sure what effect was preventing the analysis from completing, but it turned out to be the maximum activation distance.)

[Anonymous]

Hi John 🙂
Its almost ok, with the constraints. Thank you for your time.

I totally misunderstood the constraints in the 1st post - i thought that you wanted me to assign them into the bottom part of the assembly, the inner axial surface - therefore I got confused and brought a post about the cylinder. 

The mistake with the enforced motion - I apologize it was probably inattention. 

The biggest challenge for me is the contact setup in the non - linear option. As i am trying to analyze the different geometry and the analyze is not converging even though the setup is identical. Do you  have any guide or contact handbook or something like this as I went through autodesk center / autodesk mechanical sim and there are no good examples of more advanced analyses. 

Do you think that if we perform a transient simulation will it be similar to explicit one and would better reflect the behavior of the part ?
Thank you !




Than