WORKSHOP 7 PARASOLID SOLID EXAMPLE PAT301, Workshop 7, October 2003 WS7-1

WS7-2 PAT301, Workshop 7, October 2003

WS7-3 PAT301, Workshop 7, October 2003 n Problem Description u Create a parasolid solid model of a tension fitting. This is done using some of the parasolid tools in MSC.Patran, e.g. boolean. Create a tet10 solid element mesh model, including the needed load and constraint, material and element properties, and analysis input. Run the finite element analysis using MSC.Nastran. Then, display the deformation and stress results in Patran.

WS7-4 PAT301, Workshop 7, October 2003 n Suggested Exercise Steps 1. Create a new database for the tension fitting model. 2. Create all the necessary 2D Geometry. 3. Extrude the surface to begin creating the solid model. 4. Create a solid shell by removing part of the solid. 5. Create fillets for all inside edges of the solid. 6. Create holes for the model by creating solid cylinders that pass through it, and then use boolean to subtract the cylinders. 7. Create cylinders to imprint the model. 8. Imprint the solid using the cylinders. 9. Delete the cylinders used for imprinting. 10. TetMesh the completed solid 11. Create loads and constraints on the model that will be used in the analysis. 12. Create material properties for the model. 13. Create the 3D element properties. 14. Check to see that the load case Default has the load and constraint. 15. Run the analysis by sending the model to MSC.Nastran. 16. Access the results by attaching the XDB file. 17. Post-process the results from MSC Nastran.

WS7-5 PAT301, Workshop 7, October 2003 Step 1. Create New Database for Tension Fitting Create a new database called tension_fitting.db. a. File / New. b. Enter tension_fitting as the file name. c. Click OK. d. Choose Based on Model for Tolerance. e. Choose MSC Nastran and Structural for Analysis Code and Type. f. Click OK. a b c d e f

WS7-6 PAT301, Workshop 7, October 2003 Step 2. Create Surface Create the Geometry for the tension fitting. a. Geometry : Create / Surface / XYZ. b. Enter for Vector Coordinates List. c. Enter [0 0 0] for Origin Coordinates List. d. Click Apply. a b c d

WS7-7 PAT301, Workshop 7, October 2003 Step 2. Create Surface (Cont.) Copy points at opposite corners. a. Click increase Point Size icon to show all points enlarged. b. Geometry : Transform / Point / Translate. c. Enter for Translation Vector. d. Select top-left corner and click Apply. e. Enter for Translation Vector. f. Select bottom-right corner and click Apply. a b ce d f

WS7-8 PAT301, Workshop 7, October 2003 Step 2. Create Surface (Cont.) Create a curve by connecting the two translated points and break the surface with the curve. a. Geometry : Create / Curve / Point. b. Click on one of the two points from translation as the starting point and the other as the ending point. a b b

WS7-9 PAT301, Workshop 7, October 2003 Step 2. Create Surface (Cont.) Break the surface and delete the upper portion of the original surface. a. Geometry : Edit / Surface / Break. b. Turn Auto Execute off. c. Select the rectangular surface for the Surface List and the sloped curve for the Break Curve List. d. Click Apply and Yes when message box appears. e. Click the Refresh Graphics icon. a c d e b

WS7-10 PAT301, Workshop 7, October 2003 Step 2. Create Surface (Cont.) Delete the upper surface (above the break curve). a. Geometry : Delete / Surface. b. Click on the triangular surface for the Surface List. c. Click Apply. a b c

WS7-11 PAT301, Workshop 7, October 2003 Create a parasolid solid by extruding the surface in the z-direction. a. Geometry : Create / Solid / Extrude. b. Make sure TetMeshable solid icon is selected. c. Enter for the Translation Vector. d. Select Surface 2 in the Surface List Box. e. Click Iso1 view. f. Click the Smooth- shaded icon. Step 3. Extrude the Surface to Create Solid a b c d e f

WS7-12 PAT301, Workshop 7, October 2003 Step 4. Create a solid shell Edit the solid using the shell method to create a shelled solid. a. Geometry : Edit / Solid / Shell b. Enter 0.25 for Thickness. Turn off Auto Execute. c. Click on Solid Face List and hold down the shift button and select the top, sloped, and front faces of the solid. d. Click Apply. a b d c c

WS7-13 PAT301, Workshop 7, October 2003 Step 5. Create Fillets Create the fillets on the inner edges of the solid. a. Geometry : Edit / Solid / Edge Blend. b. Make sure that the constant radius icon is selected. c. Enter 0.25 for Constant Radius. d. Make sure Edges of Solid icon is selected. e. Turn Auto Execute Off. f. Click on Solid Edge List and use the shift-click technique and select the 5 edges on the inside of the solid. g. Click Apply. It may be necessary to rotate the object in order to see then inner edges more easily. This can be done by holding the middle mouse button and moving the mouse. a b c d g f e e

WS7-14 PAT301, Workshop 7, October 2003 Step 6. Create Holes for the Tension Fitting Create the holes for the tension fitting by creating primitive solids that pass through the solid, then subtracting them. a. Geometry : Create / Solid / Primitive. b. Select the cylinder icon c. Enter 2.0 for the Height and 0.25 for the radius. d. Enter [ ] for the Base Center Point List and Coord 0.1 for the Axis List. e. Click Apply. f. Geometry : Edit / Solid / Boolean. g. Select Subtract icon. h. Select the tension fitting for the Target Solid. i. Select the cylinder for the Subtracting Solid List. a b c d e f g h i

WS7-15 PAT301, Workshop 7, October 2003 Step 6. Create Holes for the Tension Fitting (Cont.) Create the points where the three bottom holes will be placed by translating an existing point and, then translating again. a. Click wireframe icon. b. Geometry : Transform / Point / Translate. c. Enter for Translation Vector. d. Select point at base edge of fillet. e. Enter for Translation Vector. f. Select translated point g. Enter for Translation Vector. h. Enter 2 for repeat count. i. Select translated point. a b c d f h i

WS7-16 PAT301, Workshop 7, October 2003 Step 6. Create Holes for the Tension Fitting (Cont.) Create cylinders using points as base centers and then create holes by subtracting them from the solid. a. Click Smooth shaded icon. b. Geometry : Create / Solid / Primitive. c. Select cylinder icon. d. Enter -1.0 for Height List and for Radius List. e. Use the shift-click technique to select the three translated points for Base Center Point List. f. Enter Coord 0.2 for axis list and click Apply. g. Geometry : Edit / Solid / Boolean. h. Select subtract icon i. Select tension fitting as Target Solid. j. Shift-click all three cylinders for Subtracting Solid List. k. Click Apply. It may be necessary to rotate the object several times in order to select the cylinders with ease b c d e f g h i j k j a

WS7-17 PAT301, Workshop 7, October 2003 Step 7. Create Cylinders to Imprint Tension Fitting Create a point in the center of the big hole in order to create the cylinder to imprint onto the solid. Then create all four cylinders that will be used for Imprinting. a. Click wireframe icon. b. Geometry : Create / Point / ArcCenter. c. Select the larger hole edge. d. Geometry : Create / Solid / Primitive. e. Select cylinder icon f. Enter 1.0 for Height and for Radius. g. Click on point in the center of the big hole. h. Enter Coord 0.1 for Axis List. i. Click Apply. j. Select Smooth Shaded icon. a bcd e f g h i j c g

WS7-18 PAT301, Workshop 7, October 2003 Step 7. Create Cylinders to Imprint Tension Fitting (Cont.) Now, create the three cylinders that will be used to imprint the base of the tension fitting. a. Click wireframe icon. b. Geometry : Create / Solid / Primitive. c. Select cylinder icon d. Enter 0.5 for Height and for Radius. e. Shift-click on point in the center of each of the base holes. f. Enter Coord 0.2 for Axis List. g. Click Apply. h. Select Smooth Shaded icon. a b c d e f g h

WS7-19 PAT301, Workshop 7, October 2003 Step 8. Imprint the Solid Use the cylinders to imprint the solid and then delete the cylinders, resulting in the finished solid. a. Geometry : Edit / Solid / Imprint. b. Turn off Auto Execute. c. Select the tension fitting for the Solid List. d. Shift-click all four cylinders under Solid to Imprint List. e. Click Apply. The solid may seem unchanged, but the imprints on the solid will not be visible until the all the cylinders have been deleted. a b c e d

WS7-20 PAT301, Workshop 7, October 2003 Step 9. Delete the Cylinders Delete the cylinders and make sure imprint method was completed. a. Geometry : Delete / Solid b. Shift-click all four cylinders for Solid List. c. Click Apply. The imprints created from the previous step are now visible. Imprinting is used to show where washers on an object will be placed. It allows for application of a total load over the imprinted area, which will be performed later a b c

WS7-21 PAT301, Workshop 7, October 2003 Step 10. TetMesh the Completed Solid Create the TetMesh for the tension fitting. a. Elements : Create / Mesh / Solid. b. Make sure Tet, TetMesh, and Tet10 are all selected. c. Click on Input List and select all solid. d. Remove check for Automatic Calculation and enter 0.25 for Global Edge Length. e. Click Apply. a b c d e

WS7-22 PAT301, Workshop 7, October 2003 Step 11. Create Loads and Constraints Create the loads and constraints for the model. a.Click Smooth Shaded icon b.Loads/BCs : Create / Total Load / Element Uniform. c.Enter Force as the New Set Name. d.Click Input Data… e.Enter for the Load and click OK. f.Click Select Application Region… g.Select the vertical solid face created by imprinting at the larger hole, then click Add. h.Click OK i.Click Apply. a b c d e f g h i Illustrated here is the desired application region. g

WS7-23 PAT301, Workshop 7, October 2003 Step 11. Create Loads and Constraints (Cont.)

WS7-24 PAT301, Workshop 7, October 2003 Step 11. Create Loads and Constraints (Cont.) Create the constraints on the base holes. a. Loads/BCs : Create / Displacement / Nodal. b. Enter Fixed as New Set Name. c. Click Input Data… d. Enter for Translation only, and click OK. e. Click Select Application Region. f. Click on Select Geometry Entities. g. Select Surface or Face icon h. Shift-click the surface(inside) of the three holes on the base, and Click Add. i. Click OK. j. Click Apply. a b c d e f g h i j h Illustrated here is the desired application region for one of the three holes.

WS7-25 PAT301, Workshop 7, October 2003 Step 11. Create Loads and Constraints (Cont.)

WS7-26 PAT301, Workshop 7, October 2003 Step 12. Create Material Properties Create the material properties for the model. a. Materials : Create / Isotropic / Manual Input b. Enter Aluminum for Material Name. c. Click Input Properties… d. Enter 10E6 for Elastic Modulus and 0.3 for the Poisson Ratio. e. Click OK f. Click Apply. a b d c e f

WS7-27 PAT301, Workshop 7, October 2003 Step 13. Create 3D Element Properties Create the 3D element properties for the tension fitting. a. Properties : Create / 3D / Solid. b. Enter 3D_tets for Property Set Name. c. Click Input Properties… d. Click Mat Prop Name icon. Select Aluminum from Select Material. e. Click OK f. For Application Region, select entire solid by dragging a box around it and click Add. g. Click Apply. a b c e f g d

WS7-28 PAT301, Workshop 7, October 2003 Step 14. Check the Load Case Check the load case Default to make sure that the load and constraint are selected. a. Load Cases : Modify b. Click on the load case name Default. c. Check to see that both the load and constraints are assigned. d. Click Cancel. a b c d

WS7-29 PAT301, Workshop 7, October 2003 Step 15. Run the Analysis Run the Analysis with MSC.Nastran. a. Analysis : Analyze / Entire Model / Full Run. b. Click Translation Parameters... c. Make sure XDB and Print is selected. d. Click OK. e. Click Solution Type… f. Make sure LINEAR STATIC is selected. g. Click OK. h. Click Apply. a b c d e f g h

WS7-30 PAT301, Workshop 7, October 2003 Step 16. Access the Results Attach the XDB file and access the results. a. Analysis : Access Results / Attach XDB / Result Entities. b. Click Select Results File… c. Select tension_fitting.xdb and click OK. d. Click Apply. a b c d

WS7-31 PAT301, Workshop 7, October 2003 Step 17. Display Results Create a deformation plot a. Results : Create / Deformation. b. Select Displacements, Transitional from Select Deformation Result. c. Click Apply. a b c

WS7-32 PAT301, Workshop 7, October 2003 Step 17. Display Results (Cont.) Erase the geometry and do not show the undeformed model, so that only the deformed model is shown. a. Display : Plot/Erase… b. Click Erase under Geometry. c. Click OK. d. Click Display Attributes. e. Remove check from Show Undeformed. f. For the Render Style, choose Shaded. g. Click Apply. a b c d e g f

WS7-33 PAT301, Workshop 7, October 2003 Step 17. Display Results (Cont.) Here is the deformation plot without the undeformed plot and geometry. It is often more convenient to observe the deformation without the original shape in order to get a better view of the model.

WS7-34 PAT301, Workshop 7, October 2003 Step 17. Read Results (Cont.) Plot the von Mises stress for the model. a. Results : Create / Fringe. b. Select Stress Tensor from Select Fringe Result. c. Select Display Attributes, then set Display to Element Edges d. Click Apply. It may also be helpful to change the view several times in order to get a better visualization of the deformations. This can be done either by holding down the middle button on the mouse, or using the view icons. a b c d