Shrink Fit Analysis
In this installment of NX A to Z, I am going to explain how to do a shrink fit analysis using NX. I recognize that is an unusual topic for the first installment of NX A to Z that relates to Advanced Simulation, but I just did a project that involved a shrink fit analysis, so I figured I should do the article before I forget how to do it.
The Master Model
The master model is actually an assembly and the components involved in the analysis are shown in the image below. As you can see, there is a shaft and a hub and two keys.
The Idealized Model
The shrink fit is between the hub and the shaft.
The Idealized model is shown below. Basically, some small features were removed, fillets were removed and the shaft was trimmed to within a few inches of the hub. A WAVE linked body was created for the hub, the shaft and each key and the geometry edits were done using the Synchronous Technology tools and Trim Body. The analysis was iterative; whereby the hub outline went through several changes and the Idealized model and the Finite Element Model updated automatically without any intervention.
The Finite Element Model
All of the components were essentially extruded 2D profiles, so they were easily meshed with Hexahedral elements. The cylindrical face of the shaft was divided at each face of the hub as can be seen below (this was done in the idealized part). This was done to facilitate a free coincident mesh mating condition (the mmc symbol is circled) between the shaft and the hub. The reason for the mmc was to line up the element faces on the hub and the shaft to ensure that the friction associated with the shrink fit was calculated using the correct surface area
The Simulation File
The solver is NX Nastran and the solution is 101. Both faces of the shaft were fixed and a load was applied to smaller hole in the hub as shown below.
All that is left is to create the simulation objects need for the shrink fit analysis. The first step is to create a region for the faces involved in the shrink fit for the shaft and the arm. So right click on Regions in the Simulation Navigator and select new region.
Provide a name for the region and select the associated faces.
In the offset box, you need to provide a value for the interference that was calculated for the shrink fit (for this particular application, the radial interference was .0135”). If the interference is accounted for in the geometry of the Master Model, then the Offset can be left at 0.
The next step is to create a Surface to Surface Contact Simulation Object (mine is called Shrink Fit Contact because the dialog box inherits the name of the object after it has been saved). Select one of the regions that you already created as the source region and the other as the target region. You always want to select the region with the finer mesh as the source, but in this case, the meshes were coincident, so it didn’t matter. Input a value for the coefficient of static friction and provide the minimum and maximum distance that you want NX to look for contacting elements. NX only searches for contacting pairs of elements when the analysis is started, so if I had elements that were .35” away from each other at the start of the analysis and I expected them to be in contact once the solution converged, I would need to put in a value of at least .35 for Max Search Distance, otherwise, NX would not bother with monitoring contact between those elements. The positive and negative direction is determined using the face normal, so if I had a Min Search Distance of 0, there would be no contact pairs created because the distance between the contact regions is -.0135” relative to the face normals.
An animated displacement plot is shown below. With the exaggerated displacement, you can see that most of the shrink fit is taken by the hub and there is no slippage between the hub and the shaft. The results don’t show the keys, because these results were from a previous iteration that did not have the keys.
So that is how you do a shrink fit analysis with NX Advanced Simulation and NX Nastran.