Modeling blades with plane stress elements workflow

In the following Simcenter Nastran example workflow, the 2D model represents portions of a gas turbine engine.

1. Open a 2D part to use to model the blades.

2. Create the FEM and Simulation. Solver = Simcenter Nastran****Analysis Type = Structural****2D Solid Option = ZX Plane, Z Axis or XY Plane, X Axis

3. If necessary, position the model so that the axisymmetric portion of the model is on positive half of the axisymmetric plane. For example, for Simcenter Nastran, if you select the ZX plane, move your model so that it lies in the +X half of the plane.

4. Make the FEM the work part.

5. Stitch the edges of the model together.

6. Mesh each blade with plane stress elements.

7. Mesh the other faces in the model with axisymmetric elements. In the following example, the adjacent faces represent rotors and stators.

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

9. In the Thickness group, select a Thickness Source.To represent variable thickness, select Field.

10. Select a field that defines the blade thickness.

11. Enter a value in the Number of Instances box. Each instance represents a copy of the blade as the mesh is rotated around the rotational axis.The following example shows the part that is being modeled with plane stress and axisymmetric elements. There are 45 instances of the blade.

12. Using the above steps, define thickness and number of instances for the remaining blades.

Note:

Axisymmetric elements in Simcenter Nastran are based on a 2π representation.

If you include plane stress elements with your Simcenter Nastran axisymmetric elements, and you define your plane stress element thickness with mesh associated data, and you define the Number of Instances (NI) to be greater than 1, the software assumes that your plane stress mesh is revolved. It multiplies the thicknesses by NI when writing the Simcenter Nastran input file.

In the example above, a turbine blade is repeated 45 times around a circumference. The model uses a 2D plane stress mesh to approximate the 45 blades. This plane stress mesh is adjacent to an axisymmetric mesh. The blade thickness is variable, so the thickness is defined using a field. The Number of Instances is set to 45. When the software writes the Simcenter Nastran input file, it automatically adjusts the plane stress thicknesses on export by:

Thickness written to the input file = (Thickness defined as the mesh associated data x 45).

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Modeling blades 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 } });