Interference Fit of a Ring on a Spoked Wheel

General Questions
1

Hi PPM Forum,

I’m having trouble to get reliable results for an interference fit of a Ring on a Spoked Wheel.

I started my FEA in 2D with a solid wheel and progressed to build 3D models with increased detail including the wheel spokes gussets etc.
Each time i verified my results with Kisssoft’s interference calc.

My models:

1. 2D solid wheel* → FEA = 7.1MPa KIsssoft = 6.98MPa :white_check_mark:*

*refer to fig1

Satisfied with the result, I proceeded to do a simplistic 3D model.

2. 3D Spoked wheel (simplistic full section spokes)* → FEA = 6.39 MPa Kisssoft = 6.29 MPa :white_check_mark:

*refer to fig 2

I was satisfied with the result, but I knew I had to increase the model detail to get a better representation of the real-world application.

The contact pressure is dependent on the wheel rim & spoke section thickness. I therefore need to do a detailed FEA including accurate rim and spoke dimensions. up to this point I leveraged extrude mesh & local mesh size to control mesh size and to match nodes at the interface. This helped the solver to converge & attain accurate results. however, i know with increased model complexity my meshing options will become limited.

3. Transfinite 1/4 Model
Thinking that a structured mesh is the best way to match interface meshes i made a complete transfinite mesh.

I created a fully transfinite mesh by breaking my model in substituents before meshing. I merged the meshes & matched nodes in PPM before running the analysis.

The resulting contact pressure were 24.8MPa (about 3.5x expected) and stress discontinuities were observed at interfaces where i merged the substituent elements.

*refer to fig 3

I think the inconsistencies might be due to the mesh merging & node matching operations.
Not satisfied with this approach i made an attempt with a simpler meshing procedure.

4. Simple mesh + local mesh size at interface

With my latest attempt i used standard meshing parameters and simply controlled element size at the interface. Knowing nodes won’t match at the interface I set local size to something similar as what I used in my initial 2D models. This did not work.

The contact pressure result in 2237MPa which are orders of magnitude from expected ~6MPa.

image
image1142×1047 322 KB

I have some room to inflate the mesh further and brute force it through the solver, but I expect to run into computing limits before i attain accurate results.

Can anyone please provide some tips / guidance?

2
  1. What types (formulations) of hex elements are you using ? Keep in mind that first-order elements are typically better for contact problems.
  2. Hex elements are definitely superior when it comes to uniform contact pressure distribution.
  3. What are your contact settings - hard or linear contact ? Default stiffness ? It often needs to be changed.
  4. Mortar contact may let you obtain better CPRESS distribution, but is also problematic in terms of convergence.
  5. Make sure adjustment is disabled for contact pair. Avoid merging nodes on both sides in other ways too.
  6. Do you model the interference as initial penetration of the parts ? Theoretically, you cold override it with *CLEARANCE, but it may not always work as expected: *Clearance tò simulate an interference - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX). (there is a thread about it on this forum too)
  7. Check this thread: Interference fit analysis (2D) with strange values - Tutorial 29 FEAnalyst and maybe this one too: Interference fit implementation
  8. You could consider using submodeling to get more accurate results in the selected region.
3 Likes
3

Thank you FEAnalyst,

  1. I changed mesh to C3D8 (apart from the spokes and the hub which are Linear Tet C3D4)
    I broke up the geometry, meshed and then used Tie constraints (3mm) to unite Tet with Hex (far from contact - hope it is the correct way)
  2. Hard contact, Frictional
  3. Surface to Surface → Now changed to Mortar Contact :white_check_mark:
  4. Adjustment disabled :white_check_mark:
  5. I modeled with Initial penetration as per your Tut 29

The model gets to 0 RESID. FORCE and 0.2E-13 CORR. DISP within 10 iterations then just oscillates there.

can I reduce the convergence tolerance / How can i get it to converge?

4

C3D8R would be best, but avoid C3D4 unless they are highly refined and/or far from the areas of interest. Normally, C3D10 should be used where it’s not possible to mesh with hexahedral elements. Only hex elements are good enough with linear interpolation.

Try reducing the contact stiffness if it doesn’t converge. This formula is a very good approach: Snap-fit contact snagging problem - #17 by JuanP74 - Analysis issues - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).

As I’ve mentioned, Mortar can help with CPRESS distribution, but it very often causes non-convergence. You may need to use CalculiX 2.23 - Mortar contact’s convergence seems to be improved there.

There is an option to adjust the solver controls, but that’s the last resort. First, I would focus on contact definition adjustments.

2 Likes