WORKSHOP 3
Meshing and Property Assignment
Objectives: ■ Apply a Refined Mesh near a critical location of the model. ■ Use a coarse Global Mesh for the rest of the model. ■ Define Material and Element properties, and apply them to the model.
MSC.Nastran 120 Exercise Workbook
3-1
3-2
MSC.Nastran 120 Exercise Workbook
WORKSHOP 3
Meshing and Property Assignment
Model Description: Define a Finite Element Mesh for the Clevis Model developed earlier. Use Mesh Seed to create a Refined Mesh with a higher Mesh density near a critical area. After the Mesh is created, define Material and Element properties for the model.
Figure 3.1
Mesh Parameters 6 elements per edge L2/L1 = 0.5 Global Edge Length = 0.5
L1 L2
MSC.Nastran 120 Exercise Workbook
3-3
Suggested Exercise Steps: ■ Start MSC.Patran and open the database clevis.db. ■ Starting with an isometric view of the model, zoom in on the lower half of the clevis hole. Save this view as a named view. Use the name zoom_in. ■ To further simplify the rendering of the clevis model, turn off the display lines so only the model boundaries are shown. ■ Apply the mesh seeds to increase the mesh density in a critical area. ■ Create a finite element mesh. ■ Define material properties. ■ Define element properties.
3-4
MSC.Nastran 120 Exercise Workbook
WORKSHOP 3
Meshing and Property Assignment
Exercise Procedure: 1.
Start MSC.Patran and open the database clevis.db. File/Open... Existing Database Name:
clevis.db
OK NOTE: Whenever possible, toggle off the ❑ Auto Execute option by left clicking the check box. 1a.
Use the Viewing/Select Corners option to zoom in on the clevis model. Figure 3.2 shows which part of the model to focus on. Viewing/ Select Corners Or, use the View Corners icon: View Corners Figure 3.2
Save this view by creating a named view of the current model view. Viewing/ Named View Options... MSC.Nastran 120 Exercise Workbook
3-5
Create View... zoom_in
Create New View: Apply Close 2.
To simplify the model view, turn off the display lines. Display/Geometry... Number of Display Lines:
0
Apply Cancel Or, use the Display lines icon: Display lines 3.
Create mesh seeds to increase the mesh density in the critical area.
◆ Finite Elements Action:
Create
Object:
Mesh Seed
Type:
One Way Bias
◆ Num and Elems and L2/L1 Number:
6
L2/L1:
2
In the Curve List box, choose the Curves as shown in Figure 3.3.
3-6
MSC.Nastran 120 Exercise Workbook
Meshing and Property Assignment
WORKSHOP 3
Figure 3.3.
T 1
Curves for mesh seeding. R
Z
Y
X
Z
Apply Number:
6
L2/L1:
0.5
In the Curve List box, choose the curves as shown in Figure 3.4. Figure 3.4
T 1 Z
R
Curves for additional mesh seeds.
Y
Z
X
Apply
MSC.Nastran 120 Exercise Workbook
3-7
Zoom out to see the entire model. Viewing/Fit view Or, use the Fit View icon: Fit view 4.
Create a finite element mesh.
◆ Finite Elements Action:
Create
Object:
Mesh
Type:
Solid
Global Edge Length:
0.5
Solid List:
Solid 1:22
Apply
The complete mesh should resemble Figure 3.5. Figure 3.5
T 1 Z
R
Y
Z
5.
X
Check the model for Free Edges using the verify action in the Finite Elements menu. ◆ Finite Elements
3-8
Action:
Verify
Object:
Element
MSC.Nastran 120 Exercise Workbook
WORKSHOP 3
Meshing and Property Assignment Type:
Boundaries
◆ Free Edges Apply 6.
The Free Edge plot is shown in Figure 3.6. Since the model has “cracks” or free edges, use the Equivalence tool to connect the mesh. Figure 3.6
◆ Finite Elements Action:
Equivalence
Object:
All
Type:
Tolerance Cube
Apply 7.
Re-check for free edges in the model, ◆ Finite Elements Action:
Verify
Object:
Element
Type:
Boundaries
◆ Free Edges Apply MSC.Nastran 120 Exercise Workbook
3-9
Figure 3.7 shows a free edge plot of the complete mesh without disconnected regions, or “cracks”. Figure 3.7
8.
Define material properties.
◆ Materials Action:
Create
Object:
Isotropic
Method:
Manual Input
Material Name:
steel
Input Properties... Constitutive Model:
Linear Elastic
Elastic Modulus =
30E6
Poisson Ratio =
0.3
OK Apply 9.
Define element properties.
◆ Properties
3-10
Action:
Create
Object:
3D
Type:
Solid
MSC.Nastran 120 Exercise Workbook
WORKSHOP 3
Meshing and Property Assignment Property Set Name:
solid_elements_steel
Input Properties... Material Name:
m:steel
OK Select Members:
Solid 1:22
Add Apply
Quit MSC.Patran after finishing this exercise.
MSC.Nastran 120 Exercise Workbook
3-11
3-12
MSC.Nastran 120 Exercise Workbook