Model Bolt Preloads in Femap with a Solid Element Approach11 May, 2016 By: Alastair Robertson
Femap Tips and Tricks: With the help of NX Nastran, you can achieve a more detailed stress recovery in and around the bolt locations.
Editor's note: This tutorial courtesy of Siemens PLM.
There have been methods of modeling bolt preloads in a finite element model for many years. Some methods involved the application of compression loads to beam elements that represent the bolts, or applying a thermal loading such that the beams contract to create the desired preloading effect. NX Nastran includes more direct methods that can apply the desired compression loading directly to beams or solid elements. In this tutorial, we’ll take a look at the solid element approach, which allows for a more detailed stress recovery in and around the bolt locations.
We’ll use a simple clamp model which consists of two parts, with a bolt connecting them together. We’ve already set up the boundary conditions and the requisite contact definitions between the parts. So all that remains is to define the bolt preloading, and that’s done by creating a cross-section region with a preload load case.
To help with the cross-section region, let’s first define a group of the desired cross-section nodes, and we’ll choose the middle of the bolt. In the Model Info pane, right-click on Groups and select New, then enter a title. Rotate the view such that you look at the side of the bolt. In the menu, select Group / Node / ID and pick a group of nodes on the bolt that can represent a cross section.
Bolt regions can be created for bolts represented by solid elements or beam elements. To create the bolt region, right-click on Regions in the Model Info tree, and select New Bolt Region. In the Bolt Region dialog, enter a title, select the Solid radio button, and click the Add Multiple… button to select multiple nodes. In the Entity Selection – Enter Node(s) to Select dialog, pick up the group of nodes previously created. The node IDs will now populate the Bolt Region dialog. In this dialog we also need to define the bolt axis, which in this example is the y-direction, so select 2..Y in the Dir box.
Click OK to complete the bolt region definition, then Cancel.
In addition to the region, we also need to create the preload load case. This references the region, and includes the preload value, which is the specified torque translated into an axial load arising from the components being bolted together. In the menu select Model / Load / Bolt Preload…, enter a title in the resulting New Load Set dialog, and click OK. In the Create Bolt Preload dialog, enter a preload value in the Preload box; 500.0 would be suitable for this example.
Click OK and the Entity Selection – Select Region(s) for Preload dialog will appear. Enter the bolt region ID and click OK, then Cancel. For clarity in this example, the only loading that we’ll consider in the analysis is the preloaded bolt load. It is possible, however, to define further load cases and apply them in addition to the effect of the preloaded bolts.
Set up a new analysis set in the Analysis Set Manager (right-click on Analyses in the Model Info tree and select Manage).
Set the analysis to run by clicking Analyze in the Analysis Set Manager dialog.
The results can be reviewed when the analysis is completed. For this case, where only the preloaded bolts are considered, the default deformed shape and stress plot illustrate the effect of the preloaded bolt.
You can watch the video of this Femap tip on YouTube.