I am working on my master thesis and I have to simulate an assembly that includes a press-fit. I want to calculate the stress distribution in my parts so I use the solver 101. To simulate the press fit I use the surface to surface contact.
First of all I want to make some basic calculations to learn about the contact. For this I create a shaft-hub-connection to check against the results of the finite element analysis with an analytical calculation. My problem is that the results are very different in some areas. Maybe anybody can help me… I describe my approach:
First of all I create the shaft-hub-connection with nominal dimension (see picture model).
I use the free coincident – mesh mating condition and mesh both parts with an 3D swept mesh Hexa (8) (see picture mesh)
Both parts have the same material (steel). In the simulation part I defined the surface to surface contact. To create a press-fit, the hub has an offset of 0.012mm. To calculate the assembly I use the option “Inertia Relief”, so I have no stresses from my conditions.
In the post-processing are different results between NX and the analytical calculation.
For example the von Mises stress. The stress in the hub is okay between NX and the analytical calculation – 455MPa to 441MPa. The stress in the shaft is complete different between both calculations NX-100MPa ; Anlytical-189 MPa . (see picture post processing)
Have anybody an idea where is my problem?
Solved! Go to Solution.
What theoretical model are you comparing to and what assumptions are made in that model (thick wall, thin wall, sigma Z=0, etc.)?
At what location in your model are you recovering stress from the FE analysis?
You can see from the exaggarated dsisplacements in the third image that there are end effects in the FE analysis (radial deformation is not uniform along the entire length of the model).
Hey JimB, thanks for your answer!
Do you mean my analytical calculation? It was made with an calculation program for press-fit's, you can see it in picture "program". The calculation in this program was madewith the DIN 7190. The Fe-model and the geometry are the same. The outer diameter is 20mm, the inner diameter 10 mm. The length of my model is 30mm.
You can see the stress location on the new picture "stress location".
Yes the radial deformation is not uniform along the entire length... That isin't realistic or?
As I understood, you just need to tune your NX model in order to fit more or less the analytical reference. Therefore, just several suggestions.
1. Basically, you do not need any mesh mating conditions on the contact interface.
2. Use CHEXA(20) elements with midnodes instead of CHEXA(8).
3. If the model size with CHEXA(20) or a calculation time wil be important for you, then create something like a quarter model because of a cyclic symmetry.
4. Maintain a greater mesh proximity at the contact interface, e.g. by introducing a larger edge density at the relevant shaft and hub edges. Basically, the elemental streeses may vary ca. 10%-15% from element-to-element (your geometry possesses any singuratiy). If the larger gradient, you need to refine the mesh.
5. Compare the maximum von Mises stress with the yield strength to ensure that you are still in the elastic domain. 101 Solution is valid for the elastic domain only.
6. Avoid to use "elemental nodal" unaveraged equivalent stresses for the post processing. Use "elemental" representation for the further analysis.
Hope, this helps.
To learn how to solve an interference-fit problem ("Snap-Fit“, “Press-Fit“, “Overlapping“, etc) using NX NASTRAN (SOL101) analysis take a look to my blog in the following address:
Basically you need to create the geometry of the contact parts with its real geometry, mesh them using high-order elements CHEXA 20-nodes (making sure to have midside nodes moved to the geometry for sure!!) and define surface-to-surface contact using a NEGATIVE MINIMUM SEARCH DISTANCE in the contact property to capture the existing interference, this way the NX NASTRAN solver will resolve the interference fit and compute the stress results in both parts, OK?.
You can solve your problem in 2-D as well, for instance a plain strain analysis, or in 3-D using 3-D Solid elements, in this case you can study 1/4 problem in order to stabilize the solution using symmetries ...
thank you very much for all the informations.
My problem was very simple... In the surface to surface contact defination I thaught that i have to give him a "coefficient of static friction"...
In your blog Blas_Molero, i saw that you don't do anything like it. Now the calculation is right.
Thank you very much !