WS19-3 PAT301, Workshop 19, October 2003 n Problem Description u There are various methods to analyze a physical system. For this case the system is the connecting rod. The following workshop exercise will consist of analyzing the connecting rod using 2D plate elements. After the geometry(surfaces) has been imported from an existing file, it will be meshed with quad4 elements. Then, loads(on edges) and boundary conditions(constraints), and element properties(e.g. thickness) will be assigned to the 2D mesh. The model will then be analyzed using MSC.Nastran. The displacements and stress will be viewed in MSC.Patran.
WS19-4 PAT301, Workshop 19, October 2003 n Suggested Exercise Steps 1. Create a new database called connecting_rod_2D.db and import the IGES file. 2. Mesh the geometry(surfaces) using the IsoMesher with quad4 elements. 3. Connect all the elements of the model by equivalencing the nodes. 4. Create a cylindrical coordinate system at the center of the top of the connecting rod. 5. Create a field to be used with the applied edge loading. It will use the cylindrical coordinate system. 6. Create the necessary loads and boundary conditions for the model. The load will be at the top of the model(at piston) and the constraints will be at the bottom(at crank shaft). 7. Create the aluminum material properties. 8. Create the 2D plate(shell) element properties for the connecting rod. 9. Check the load case Default to insure that all the loads and boundary conditions are selected. 10. Run the simulation using MSC.Nastran. 11. Read and view the results in MSC.Patran. Both deformations and stresses will be looked at. Two different coordinate systems will be used to view the stresses.
WS19-5 PAT301, Workshop 19, October 2003 Step 1. Create a New Database and Import Geometry Create a new database called connecting_rod_2D.db and import the IGES file, conrod.igs. a. File : New. b. Enter connecting_rod_2D as the File name. c. Click OK. d. Select Default Model Preferences. e. File : Import. f. Change the Source to IGES. g. Select conrod.igs and click Apply. h. Click OK when Summary appears. a b c f g h d e
WS19-6 PAT301, Workshop 19, October 2003 Step 1. Create a New Database and Import Geometry (Cont.)
WS19-7 PAT301, Workshop 19, October 2003 Step 2. Mesh the Surfaces Mesh the connecting rod geometry using the IsoMesh mesher. a. Elements : Create / Mesh / Surface. b. Select Quad, IsoMesh, and Quad4. c. Remove check for Automatic Calculation and enter for the Global Edge Length. d. Select the entire object and click Apply. a b c d d
WS19-8 PAT301, Workshop 19, October 2003 Step 3. Equivalence the Nodes Equivalence the nodes in order to connect all the elements. a. Elements : Equivalence / All / Tolerance Cube. b. Click Apply. c. Elements : Verify / Element / Boundaries. d. Select Free Edges. e. Click Apply. c d e a b
WS19-9 PAT301, Workshop 19, October 2003 Step 4. Create a Cylindrical Coordinate System Before creating the cylindrical coordinate system, it is necessary to change the view and zoom in on a certain part of the geometry. a. Click the Iso 1 View icon. b. Increase the point size by clicking on the Point size icon. c. Click on the View corners icon and box the top portion of the surface as shown below. abc
WS19-10 PAT301, Workshop 19, October 2003 Step 4. Create a Cylindrical Coordinate System (Cont.) Now create the cylindrical coordinate system using the 3Point method. a. Geometry : Create / Coord / 3Point. b. Type : Cylindrical c. Select the center point of the piston for the Origin. d. Enter [x2 y2 1] for the Point on Axis 3 (By entering x2 and y2, this point will use the x and y coordinates of Point 2). e. Select point (as indicated) for Point on Plane 1-3. a b c d e e
WS19-11 PAT301, Workshop 19, October 2003 Step 5. Create a Field Create a field. This field will be used to create a CID Distributed Load later in this exercise. a. Fields : Create / Spatial / PCL Function. b. Enter sin_load for the field name. c. Select Vector for the field type. d. Select the cylindrical coord system (Coord 1). e. Enter sinr(T) under First Component. f. Click Apply. a b c d e f
WS19-12 PAT301, Workshop 19, October 2003 Step 6. Create Loads and Boundary Conditions Create a distributed load using the existing field. a. Loads/BCs : Create / CID Distributed Load / Element Uniform. b. Enter CID_distributed for New Set Name. c. Target Element Type : 2D d. Click Input Data… e. Enter 1000 for the Scale Factor and under Edge Distr Force, select the spatial field sin_load f. Select Coord 1 for the Analysis Coordinate Frame and click OK. g. Click Select Application Region… h. Select the 7 surface edges (indicated on next page), click Add, then OK. i. Click Apply. a b c d e f g h i
WS19-13 PAT301, Workshop 19, October 2003 Step 6. Create Loads and Boundary Conditions (Cont.) h
WS19-14 PAT301, Workshop 19, October 2003 Step 6. Create Loads and Boundary Conditions (Cont.) Create the constraint set for the model. This constraint will fix all six degrees_of_freedom at the contact area of the crankshaft. a. Click on the Fit View icon. b. Click on the View Corners icon and box the crank section (bottom portion) of the model. c. Loads/BCs : Create / Displacement / Nodal d. Enter fix_at_crank for the New Set Name. e. Click Input Data… f. Enter under Translations and Rotations, then click OK. c d f e ba
WS19-15 PAT301, Workshop 19, October 2003 Step 6. Create Loads and Boundary Conditions (Cont.) Finish creating the constraint by selecting the application region. a. Click on Select Application Region… b. Select the 6 surface inside edges (shown below) and click Add. c. Click OK. d. Then click Apply. a c d b b
WS19-16 PAT301, Workshop 19, October 2003 Step 6. Create Loads and Boundary Conditions (Cont.) These are the model constraints at the interface to the crankshaft. Six nodal dofs constrained at each node on the six edges
WS19-17 PAT301, Workshop 19, October 2003 Step 7. Create Material Properties Create a material property for aluminum. a. Materials : Create / Isotropic / Manual Input. b. Enter Aluminum for the Material Name. c. Click on Input Properties… d. Enter 10E6 and 0.3 for Elastic Modulus and Poisson Ratio, respectively. e. Click OK f. Click Apply. a b c d e f
WS19-18 PAT301, Workshop 19, October 2003 Step 8. Create Element Properties Create the element properties for the model. a. Properties : Create / 2D / Shell b. Enter 2D_crank for the Property Set Name. c. Click Input Properties… d. Click on the Material Property Name icon and select Aluminum from Select Existing Material. e. Enter for the Thickness. The thickness values are slightly different for this exercise than those for Workshop 15. f. Click OK. a b c d e f
WS19-19 PAT301, Workshop 19, October 2003 Step 8. Create Element Properties (Cont.) Select the application region for the 2D_crank property. a. Click on Application Region. For the application region, shift-select the 9 surfaces that make up the crank (the ring). b. Click Add. c. Click Apply. d. Repeat Step 8 to create three more properties: 2D_piston, 2D_flange, 2D_web. b c
WS19-20 PAT301, Workshop 19, October 2003 Step 8. Create Element Properties (Cont.) Illustrated are the application regions for each property set. Below is a table listing each property set name with its corresponding material set and thickness. Property Set NameMaterial NameThickness 2D_crankAluminum D_pistonAluminum D_flangeAluminum0.75 2D_webAluminum0.375 The red ring indicates the application region for the 2D_piston property. There should be a total of 9 surfaces that make up this ring. Six surfaces make up the application region for the 2D_flange property set. The application region is indicated in purple. Similarly, six surfaces compose the application region for the 2D_web property set. This region is indicated in white.
WS19-21 PAT301, Workshop 19, October 2003 Step 9. Check the Load Case Check the load case Default to ensure that the correct Loads/BCs are selected. a. Click on the Fit View icon. b. Load Cases : Modify c. Click on the load case name Default. d. Make sure the correct Loads/BCs are applied. e. Click Cancel. a b c d e
WS19-22 PAT301, Workshop 19, October 2003 Step 10. Run the Analysis Send the model to MSC.Nastran for analysis. a. Analysis : Analyze / Entire Model / Full Run. b. Click Translation Parameters… c. Make sure XDB and Print is selected. d. Click OK. e. Click on Solution Type… f. Make sure Linear Static is selected and click OK. g. Click Apply. a b c d e f g
WS19-23 PAT301, Workshop 19, October 2003 Step 11. Read Results Attach the XDB file and read the results. a. Analysis : Access Results / Attach XDB / Result Entities. b. Click on Select Results File. c. Select connecting_rod_2D.xdb and click OK. d. Click Apply. a b c d
WS19-24 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Create a deformation plot. a. Results : Create / Deformation. b. Select Displacements, Translational. c. Click Apply. a b c
WS19-25 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Erase the geometry and unpost the undeformed model and coordinate frame to get a better plot. a. Click on the Display Attributes icon. b. Remove the check from Show Undeformed. c. Click on the Plot/Erase icon d. Click Erase under Geometry. e. Click OK. f. Display: Coordinate Frames… g. Click Unpost All. h. Click OK. i. Click Apply. b c d e i a f g h
WS19-27 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Plot the Von Mises stresses. a. Reset Graphics b. Results : Create / Fringe. c. Select Stress Tensor. d. Make sure von Mises is selected. e. Click on the Display Attributes icon. f. Change the Display to Element Edges. g. Click Apply. The blue lines indicating the element edges overshadow the fringe colors, so it will be necessary to zoom in on the model to get a clearer view. b c d e f g a
WS19-28 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Illustrated here are several views of the von Mises stress. It is necessary to zoom in on different sections to see the stress spatial gradient.
WS19-29 PAT301, Workshop 19, October 2003 j l Step 11. Read Results (Cont.) Plot stress tensor components using two coordinate frames. a. Results : Create / Marker / Tensor. b. Select result case A1: Static Subcase. c. Select Stress Tensor. d. Under Show As:, select Component, and select components XX and YY. e. Click on Display Attributes icon. f. Click on Spectrum, then select Show Spectrum. g. Set Vector Definition / Length to Screen Scaled and enter 0.5 for the Scale Factor. h. Deselect Show Tensor Label. i. Click on Plot Options icon. j. Make sure the Coordinate Transformation is set to As is. k. Zoom into a top part of the model so that about 20 elements can be seen. l. Click on Apply. a b c e d f g i h
WS19-30 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Notice here that the stress tensor arrows are in the circumfrential direction.
WS19-31 PAT301, Workshop 19, October 2003 Step 11. Read Results (Cont.) Replot the same stress data, but use a different Coordinate Transformation. a. Click the Plot Options icon. b. Change the Coordinate Transformation to Global. c. Click Apply. Notice that now the stress tensor arrows lie in the Patran global coordinate directions. There are advantages to using various transformations.