Modeling holes and bolts with plane stress elements workflow

The following example workflow shows plane stress and axisymmetric elements used in the same axisymmetric model. Bolt and hole geometry is represented as plane stress elements with variable thickness. The thickness is derived from the geometry and the number of instances specified.

1. Open a 3D model of the axisymmetric part.

2. Create the FEM and Simulation. Set the Analysis Type to Structural.Set the 2D Solid Option to the axisymmetric plane and rotational axis. For example, in Simcenter Nastran, select the ZX plane and Z rotational axis.

3. If necessary, position the model so that the rotational axis aligns with the centerline of the part, and the section to be meshed is on positive half of the axisymmetric plane. For example, for Simcenter Nastran, if you selected the ZX plane, move your model so that the section to be meshed lies in the +X half of the plane.

4. Split the part along the axisymmetric plane.

5. Hide half of the part. Make sure that the section to be meshed is displayed and is on the positive half of the plane. For example, if the axisymmetric plane is ZX, the section must be on the +X half of the plane.

6. Create geometry on the axisymmetric plane to represent the bolts and holes. Note: In this example, the bolt geometry is included in the model, and the representation of the hole is created with the Four Point Surface command.

7. On the section cut, mesh the face representing the holes with plane stress elements.

8. Right-click the plane stress mesh for the holes and choose Edit Mesh Associated Data.

9. In the Thickness group, set Thickness Source to Hole.

10. Use the options in the Centerline Definition list to define the location of the centerline for the hole.

11. In the Number of Instances box, type the number. Each instance represents a copy of the hole as the mesh is rotated around the rotational axis.

12. Mesh the face representing the bolts with plane stress elements.

13. Right-click the plane stress mesh for the bolts and choose Edit Mesh Associated Data.

14. In the Thickness group, from the Thickness Source list, select Bolt.

15. In the Number of Instances box, type the number. Each instance represents a copy of the bolt as the mesh is rotated around the rotational axis.

16. Mesh the remainder of the section with axisymmetric elements.

When you solve the model, Simcenter Nastran subtracts the material in the hole's plane stress mesh from the material for the remainder of the model. The software then adds the material in the bolt's plane stress mesh back to the model.

Tip:

To display the hole’s centerline, select the Display Centerline check box in the Mesh Display dialog box.

To change the orientation of the hole’s centerline, use the Transpose Centerline option on the Mesh Associated Data dialog box.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Modeling holes and bolts with plane stress elements workflow, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });