In this tutorial, you will learn how to use the 2D Dependent Mesh command.
On your desktop or the appropriate network drive, create a folder named impeller.
Click the link below:
Extract the file to your impeller folder.
Start Simcenter 3D or NX.
Open impeller_fem1.fem.
The options you select in dialog boxes are preserved for the next time you open the same dialog box within a given session. Restore the default settings to ensure that the dialog boxes are in the expected initial state for each step of the activity.
File |
Preferences→User Interface
Options |
Reset Dialog Memory
OK |
|
The solid body of the impeller has been trimmed to a single blade. You will edit the FEM file to set the global cyclic coordinate system, a cylindrical coordinate system whose Z-axis defines the default axis of rotation for your FEM.
Simulation Navigator
impeller_fem1.fem
Edit
Default Cyclic Symmetry Cylindrical CSYS |
|
Use Cyclic CSYS if Defined
Specify CSYS |
CSYS of Object |
OK |
|
Mesh Collector (Home tab→Properties group)
Element Family |
3D |
Collector Type |
Solid |
Create Physical (Solid Property)
Name |
Aluminum |
Choose material (Material)
Materials |
|
Aluminum_2014 |
OK |
all dialog boxes |
For cyclic symmetry, the radial, tangential, and axial displacements relative to the axis of rotation are identical at equivalent positions on the repeated faces (the faces created during the trimming operation). To model this behavior:
Create a 2D dependent mesh on the repeated faces. Doing so locates the nodes on each face at equivalent positions.
Use the 2D dependent mesh to seed a 3D mesh of the body.
Change the nodal displacement coordinate system to the global cyclic analysis coordinate system.
Couple the degrees of freedom (DOF) for each pair of equivalently positioned nodes lying on the repeated faces.
2D Dependent (Mesh group→More list)
Type |
Symmetric |
Selecting the first face automatically selects the second face and the appropriate edges.
Mesh Type |
Free Mesh |
OK |
|
The 2D Mesh dialog box appears. Do not close it.
The 2D Mesh dialog box is open from the previous step.
Type |
CTRIA6 |
Element Size |
0.6 |
Mesh Settings |
|
Export Mesh to Solver
OK |
|
3D Tetrahedral (Mesh group)
Type |
CTETRA(10) |
Element Size |
0.6 |
Destination Collector |
|
Automatic Creation
The Solid(1) mesh collector that you created earlier should be automatically selected in the Mesh Collector list.
OK |
|
Save
File |
Close→All Parts