In this tutorial, you will create a time-dependent enforced displacement constraint using a table field.
On your desktop or the appropriate network drive, create a folder named plug.
Click the link below:
Extract the file to your plug folder.
Start Simcenter 3D or NX.
Open plug_sim.sim.
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 |
|
Use the Simulation Navigator to explore the existing model.
The model contains a two-body part that resembles a snap-in plug connector. You will use a large-displacement nonlinear solution to simulate the assembly of the connector.
The Simcenter Nastran structural solution type is SOL 601, 106 Advanced Nonlinear Statics.
In the Simulation Navigator, the solution's Simulation Objects container lists two face contact objects.
The contact graphics are displayed in the graphics window. The source faces for the contact are on the plug, and the target faces are on the socket.
These contact simulation objects model the regions where the plug will contact the socket as the plug is displaced.
For this solution, modify the number of time steps and time increment.
If you do not have the Simcenter Nastran Structural SOL 601,106 Advanced Nonlinear Statics solver installed, skip to the next section, Apply a time-dependent enforced displacement constraint.
Modeling Objects (Home tab→Properties group)
Selection |
|
Time Step1 |
Edit
Time Step Interval |
|
Number of Time Steps |
20 |
Time Increment |
0.05 |
The default units are seconds.
OK |
Time Step dialog box |
Close |
Modeling Objects Manager dialog box |
Simulation Navigator
plug_fem.fem
3D Collectors (hide)
Hiding the 3D meshes makes it easier to select the polygon face at the base of the socket.
Enforced Displacement Constraint (Loads and Conditions group→ Constraint Type list)
Type |
Components |
Type Filter (Top Border bar) |
Mesh Point |
the mesh point at the top of the plug
Direction |
|
Displacement CSYS |
Existing |
Degrees of Freedom |
|
DOF1 |
0 |
DOF2 |
0 |
DOF4 |
0 |
DOF5 |
0 |
DOF6 |
0 |
(DOF3)
New Field→Table
Name |
Plug Motion |
Domain |
|
Independent |
Time |
Data Points |
|
The table has three columns: Row ID, time (s), and length (mm).
(box under the table) |
0,0; 1,-21 |
Use commas to separate values in a row, and use semicolons to separate rows.
Accept Edit
The table displays displacement values at two different times:
Row ID |
time (s) |
length (mm) |
1 |
0 |
0 |
2 |
1 |
-21 |
OK |
Table Field dialog box |
(DOF3)
Plot XY
Create New Window (Viewport dialog box)
Graph Window 1
OK |
Enforced Displacement Constraint dialog box |
The enforced motion is defined at the mesh point.
Save
At this point, if the Simcenter Nastran SOL 601, 106 Advanced Nonlinear Statics solver is installed, you can solve the model.
File |
Close→All Parts