WORKSHOP 6 FRAME SURFACE MODEL ANALYSIS
z
Workshop Objectives z
z
z
Perform an analysis of the model, and postprocess the results from the analysis. The results that are looked at are 1) deformation deformation,, 2) von Mises stress stress fringe, fringe, and 3) marker tensor tensor using two different coordinate system transformations.
Problem Description z z
z
Create a finite element model (meshes; connect adjacent elements; apply dead loads, operating loads, and gravity loads; constrain nodes) for a intermediately difficult frame system using MSC.Patran
Compare stress for different transformations Frame material: Aluminum with E = 10 x 10 6 psi, ν = 0.3, and density = 2.61 x 10 -4 lbf*sec2/in4
Software Version z
MSC.Patran 2005r2 MSC.Nastran 2005r2b
z
Key Concepts and Steps: z
z z
z
z z z
z z
Database: create a new database with Analysis Code = MSC.Nastran and Analysis Type = Structural Geometry: open MSC.Patran database to access the surface geometry Elements: mesh the surfaces with the Paver mesher, connect the adjacent elements, and determine the aspect ratio of the elements Loads/BCs: constrain the four corners of the frame, and apply Total load and gravity loading to the model Materials: specify an isotropic material for Aluminum Properties: create a 2D plate/shell property Analysis: Solution Type = Nastran Linear Static, Solution Sequence = 101, Method = Full Run Analysis: access analysis results by attaching the XDB file to database Results: plot deformatio deformation, n, von Mises stress, stress, and marker tensor tensor results. results. Use two different coordinate system transformations for the marker tensor results.
Step 1. Open Database surf_create_part2.db
a
a. File / Open. b. File name: surf_create_part2. c. Click OK.
b
c
Step 2. Create Group for 2D Paver Meshes a
a. Group / Create. b. New Group Name: fem_surfaces. c. Check Make Current. d. Apply. e. Cancel.
b
c
d
e
Step 3. Create Paver Mesh for All Surfaces
a a. Elements: Create / Mesh / Surface.
e
b. Elem Shape: Quad. c. Mesher: Paver .
b c d
d. Topology: Quad4. e. Click under Surface List and select all surfaces in the figure, Surface 1:182. f.
Global Edge Length: 1.0.
g. Apply.
e f
Step 3. Create Paver Mesh for All Surfaces (Cont.)
These are the Paver meshes, one for each of the 182 surfaces.
Step 5. Equivalence Nodes
a. Elements: Equivalence / All / Tolerance Cube. b. Equivalencing Tolerance: 0.005. c. Apply.
a
b c
Step 6. Show Element Free Edges
a. Elements: Verify / Element / Boundaries. b. Display Type: Free Edges. c. Apply.
a
b
c
Step 9. Verify Elements
a
b a. Elements: Verify / Quad / Aspect. b. Aspect Ratio: 5. c. Apply.
c
Step 10. Post Group “all_surfaces”
a
a. Group / Post. b. Under Select Groups to Post select all_surfaces. c. Apply. d. Cancel.
b
Step 11. Create Dead Load from Engine b a
a. Change view to Smooth shaded. b. Zoom into the area as shown in the figure.
b
Step 11. Create Dead Load from Engine (Cont.)
a
g
a. Loads/BCs: Create/ Force/Nodal.
d
b. Select on New Set Name and enter dead_load. c. Input Data. d. Enter <0 -150 0> for Surf Load
.
h
e. OK. f.
Select Application Region.
g. Geometry Filter: Geometry. h. Select on Select Geometry Entities.
c f
e b
Step 11. Create Dead Load from Engine (Cont.)
a. Select points as shown in the figure.
a
b. Add. c. OK. d. Apply.
a a
b
c
Step 11. Create Dead Load from Engine (Cont.)
a. Change to the model region shown in the figure.
a
Step 11. Create Dead Load from Engine (Cont.)
f
a. Select on New Set Name and enter dead_load_2.
c
b. Input Data. c. Enter <0 -960 0> for Surf Load . d. OK.
g
e. Select Application Region. f.
Geometry Filter: Geometry.
g. Select on Select Geometry Entities.
b e
a
d
Step 11. Create Dead Load from Engine (Cont.)
a
a. Select points as shown in the figure. b. Add. c. OK. d. Apply.
a b
c
a
Step 11. Create Dead Load from Engine (Cont.)
a. The figure should look like the following. b. Zoom out.
b a
Step 12. Create Operating Engine Static Load
f
a. Select on New Set Name and enter op_static_load.
c
b. Input Data. c. Enter <0 -100 -100> for Surf Load . d. OK. e. Select Application Region. f.
g
Geometry Filter: Geometry.
g. Select on Select Geometry Entities.
b e
a
d
Step 12. Create Operating Engine Static Load (Cont.)
a. Select points as shown in the figure. b. Add.
a
c. OK. d. Apply.
a a
b
c
Step 12. Create Operating Engine Static Load (Cont.)
a. The figure should look like the following.
Although the force directions may appear vertical, they are in fact off angled. Different views can be used to observe this.
Step 13. Create Gravity Load on Frame
a a. Loads/BCs: Create/Inertial Load/Element Uniform
d
b. Enter gravity for New Set Name. c. Input Data. d. In Trans Accel enter <0 –386.4 0>. e. OK. f. Apply.
c
b
Step 14. Create Constraints for the Frame Support
g
a
Constrain at the corners of the frame.
d
a. Loads/BCs: Create/ Displacement/Nodal. b. Select on New Set Name: and enter fix_base. c. Select Input Data. d. Enter <0 0 0> for Translations . e. OK. f.
Click on Select Application Region.
g. Select Geometry for Geometry Filter .
c f
b
e
Step 14. Create Constraints for the Frame Support (Cont.)
c
a. Click under Select Geometry Entities. b. Pick the Points icon. c. Change to wireframe. d. Select the four points as shown. e. Add. f. OK. g. Apply.
d
b
a e
d f
Step 14. Create Constraints for the Frame Support (Cont.)
a b a. Select on Iso 1 View from the tool bar. b. Display / Load/BC/Elem.Props. c. Unselect Show LBC/El.Prop. Values. d. Apply. e. Cancel. f. The figure should look like the following.
f
c
d
e
Step 15. Defining Material
a Set aluminum as the material of the frame.
d
a. Materials: Create / Isotropic / Manual Input. b. Select on Material Name and enter aluminum. c. Select Input Properties. d. Enter: Elastic Modulus: 10e6. Poisson Ratio: 0.3. Density: 2.61e-4.
b
e. OK. f. Apply.
c e
Step 16. Defining Properties for Frame Structure
a a. Properties: Create / 2D / Shell.
d
b. Select Property Set Name and enter alframe_flange.
e
c. Select Input Properties. d. Click on Mat Prop Name select aluminum from Select Material.
b
e. Thickness: 0.75. f.
OK.
c
f
d
Step 16. Defining Properties for Frame Structure (Cont.)
a
b
a. Change view to Front View. b. Click on Preferences/Picking.
e
c. Change to enclose entire entity. d. Click on Select Members. e. Select top and bottom flanges as shown in the figure. f. Add. g. Apply.
d f
Select flange surfaces
Step 16. Defining Properties for Frame Structure (Cont.) a
a. Preferences / Picking.
f
b. Rectangle/Polygon Picking: Enclose any portion of entity.
g
c. Close. d. Select Property Set Name and enter al_frame_web. e. Select Input Properties. f.
Click Mat Prop Name icon and choose aluminum from Select Material.
g. Thickness: 0.5.
d
h. OK.
e
h
f
Step 16. Defining Properties for Frame Structure (Cont.)
a. Click on Select Members. b. Select the web surfaces(between flanges; trimmed surfaces with holes) of the frame as shown in the figure.
b
Select web surfaces
c. Add. d. Apply.
Flange surface
a c
Step 17. Check Assignment of Loads and BC’s to Load Case
a a. Load Cases: Modify. b. Select Default in Select Load Case to Modify . c. Check that all Loads and BC’s are selected.
b
d. Cancel.
c
Step 18. Post Group “fem_surfaces”
a
a. Group / Post. b. Under Select Groups to Post select fem_surfaces. c. Apply. d. Cancel.
Step 19. Analysis
a Run the analysis of the entire model.
c
a. Analysis: Analyze / Entire Model / Full Run. b. Select Solution Type. c. Choose LINEAR STATIC for Solution Type. d. OK. e. Apply.
b
e
d
Step 20. Access Results Under Analysis
a
Attach the .xdb file in order to access the results. a. Analysis: Access Results/ Attach XDB/Result Entities. b. Click on Select Results File.
c
c. Select and attach the file surf_create_part2.xdb.
d
d. OK. e. Apply.
b
Step 21. Deformation Results
a Create a deformed shape plot . a. Results: Create / Deformation. b. Select A1:Static Subcase under Select Result Case(s).
d b
c. Select Displacements, Translational under Select Deformation Result . d. Select Display Attributes. e. Click on Model Scale and set the scale to 0.01. f.
Unselect Show Undeformed.
g. Apply.
c f
e
Step 21. Deformation Results (Cont.)
Display shows the deformed shape of the structure.
Step 21. Deformation Results (Cont.)
a. Render Style: Shaded. b. Apply.
a
b
Step 22. Stress Fringe Results
a a. Create / Fringe. b. Select Stress Tensor under Select Fringe Result .
d
c. Select Position…((NONLAYERED)). d. Choose At Z1. e. Close. f.
Quantity: von Mises.
g. Apply.
b
c f g
e
Step 22. Stress Fringe Results (Cont.)
a. The figure should look like the following.
Step 23. Stress Marker Results
a
b
a. Reset graphics. b. Create / Marker / Tensor. c. Select Stress Tensor under Select Fringe Result .
h
d. Select Position…((NONLAYERED)).
k
e
e. Choose At Z1. f.
Close.
c
g. Check only XX and YY. h. Display Attributes. i.
Uncheck Show Max/Min Label .
j.
Uncheck Show Tensor Label .
k. Plot Options. l.
Coordinate Transformation: As Is.
d g
i
m. Apply.
m
f
j
Step 23. Stress Marker Results (Cont.)
a. Zoom in to the figure shown. b. The markers are for XX and YY components of stress using the coordinate transformation As Is (no transformation).
Step 23. Stress Marker Results (Cont.)
a
a. Reset graphics. b. Plot Options. c. Coordinate Transformation: Global.
b c
d. Apply.
d
