PAT301, Workshop 1, October 2003 WS1-1 WORKSHOP 1 PISTON HEAD ANALYSIS

WS1-2 PAT301, Workshop 1, October 2003

WS1-3 PAT301, Workshop 1, October 2003 n Problem Description u This is an introductory exercise that will utilize the basic tools and capabilities of MSC.Patran. A preliminary design for a piston will be imported and analyzed to verify whether or not the design can withstand the expected loads.

WS1-4 PAT301, Workshop 1, October 2003 n Suggested Exercise Steps 1. Create a database piston.db. 2. Import the existing geometry. 3. Create a finite elemental mesh for the piston head. 4. Use the Plot/Erase feature to erase the geometry. 5. Create a nodal constraint at each of the pinhole surfaces of the model. 6. Create a uniform pressure load applied to the top surface of the piston. 7. Create the material property for steel. 8. Create a 3D element property for the model. 9. Check the load case Default and verify that the correct loads and boundary conditions have been applied. 10. Send the model to MSC.Nastran to be analyzed. 11. Read the results.

WS1-5 PAT301, Workshop 1, October 2003 Step 1. Create a New Database Create a new database called piston.db and set the model preferences. a. File / New. b. Enter piston.db for the File Name. c. Click on OK. d. Set the Tolerance under Model Preferences to Based on Model. e. Make sure that the Analysis Code and Analysis Type are set to MSC.Nastran and Structural, respectively. f. Click on OK. a bc d e f

WS1-6 PAT301, Workshop 1, October 2003 Step 2. Import the Model Geometry Import the model geometry. a. File / Import b. Make sure Source is set to Parasolid.xmt. c. Select piston.xmt. d. Click on Apply. e. Click on OK when Import Summary form appears. f. Click on Smooth Shaded icon and Top View icons. g. Use the middle mouse button and rotate the model to attain the same view shown on next page. a b c d f

WS1-7 PAT301, Workshop 1, October 2003 Step 2. Import the Model Geometry (Cont.)

WS1-8 PAT301, Workshop 1, October 2003 Step 3. Create a Finite Element Mesh Create a finite element mesh for the model using the TetMesh-er. a. Elements : Create / Mesh / Solid. b. Set Elem. Shape, Mesher, and Topology to Tet, TetMesh, and Tet10, respectively. c. Select Solid 1 under Input List. d. Uncheck Automatic Calculation and enter 0.5 for the Global Edge Length. e. Click on Apply. a b c e d

WS1-9 PAT301, Workshop 1, October 2003 Step 5. Create Constraints Constrain the two pinhole surfaces. a. Loads/BCs : Create / Displacement / Nodal. b. Enter fixed for the New Set Name. c. Click on Input Data… d. Enter under Translations only. e. Click on OK. a b c d e

WS1-10 PAT301, Workshop 1, October 2003 Step 5. Create Constraints (Cont.) Select the application region for the nodal constraints. a. Click on Select Application Region… b. Set the Geometry Filter to Geometry. c. Click under Select Geometry Entities, then on the Surface or Face icon. d. Select both pinhole surfaces and click Add. e. Click on OK. f. Click on Apply. a b d e g c Illustrated above are the two application regions for the model. After choosing the first application region and clicking Add, use the middle-mouse button to rotate the model and select the other pinhole surface. c d

WS1-11 PAT301, Workshop 1, October 2003 Step 6. Create a Pressure Load Create a pressure that will be applied to the top surface of the piston. a. Loads/BCs : Create / Pressure / Element Uniform. b. Enter piston_pressure for the New Set Name. c. Click on Input Data… d. Enter for the Pressure. e. Click on OK. a b c d e

WS1-12 PAT301, Workshop 1, October 2003 Step 6. Create a Pressure Load (Cont.) Select the application region for the pressure. a. Click on Select Application Region… b. Set the Geometry Filter to Geometry. c. Click under Select Solid Faces, then select the top face of the piston, and click Add. d. Click on OK. e. Click on Apply. a b c d e Shown above is the application region for the pressure load. c

WS1-13 PAT301, Workshop 1, October 2003 Step 6. Create a Pressure Load (Cont.) It may not seem as though the pressure load is applied uniformly throughout the top surface of the piston. That is because the application region was geometry, and not FEM. When this is done the markers only appear at geometry display lines.

WS1-14 PAT301, Workshop 1, October 2003 Step 7. Create Material Properties Create a material property for the piston. a. Materials : Create / Isotropic / Manual Input. b. Enter steel for the Material Name. c. Click on Input Properties… d. Enter 30E6 and 0.3 for the Elastic Modulus and Poisson Ratio, respectively. e. Click on OK. f. Click on Apply. a b c d e f

WS1-15 PAT301, Workshop 1, October 2003 Step 8. Create Element Properties Create a 3D element property for the model. a. Properties : Create / 3D / Solid. b. Enter piston for Property Set Name. c. Click on Input Properties… d. Click on Mat Prop Name icon Choose steel from Select Material. e. Click on OK. f. Click on Select Members and select Solid 1. g. Click on Add. h. Click on Apply. a b c d e f g h

WS1-16 PAT301, Workshop 1, October 2003 Step 9. Check the Load Cases Check the load case Default and verify that the correct loads and boundary conditions are being applied. a. Load Cases : Modify b. Click on the Default load case. c. Check to see that the correct loads are assigned and click Cancel. a b c

WS1-17 PAT301, Workshop 1, October 2003 Step 10. Run the Analysis Send the model to MSC.Nastran and analyze the model. a. Analysis : Analyze / Entire Model / Full Run. b. Click on Translation Parameters… c. Set Data Output to XDB and Print. d. Click on OK. e. Click on Solution Type… f. Set Solution Type to Linear Static and click OK. g. Click on Apply. f e g b a c d

WS1-18 PAT301, Workshop 1, October 2003 Step 11. Read the Results Read in the results file into MSC.Patran by attaching the XDB file. a. Analysis : Access Results / Attach XDB / Result Entities. b. Click on Select Results File… c. Select piston.xdb and click OK. d. Click on Apply. a b c d

WS1-19 PAT301, Workshop 1, October 2003 Step 11. Read the Results (Cont.) Plot both the deformation and the stress tensor using quick plot. a. Click on the Plot/Erase icon. b. Click on Erase under Geometry. c. Click on OK. d. Results : Create / Quick Plot. e. Select Stress Tensor and Displacements, Translational from Select Fringe Result and Select Deformation Result, respectively. f. Make sure that the Quantity is set to von Mises. g. Click on Apply. d f g e a b c

WS1-20 PAT301, Workshop 1, October 2003 Step 11. Read the Results (Cont.) Modify the deformation attributes. a. Click on the Deform Attributes icon. b. Uncheck Show Undeformed and Show Title. c. Click Apply. d. Click on the Plot/Erase icon. e. Click on Erase under Geometry. f. Click on OK. c a b d

WS1-21 PAT301, Workshop 1, October 2003 Step 11. Read the Results (Cont.) Modify the fringe attributes. a. Click on the Fringe Attributes icon. b. Set Display to Element Edges. c. Uncheck Show Title. d. Click on Apply. b c d a

WS1-22 PAT301, Workshop 1, October 2003 Step 11. Read the Results (Cont.) Illustrated here is the complete model deformation and stress fringe plot.