ME 5510/6510 INTRODUCTION TO FINITE ELEMENTS AUTUMN 2005 This Lab deals with the following: 1. Importing a solid model (iges file) into ANSYS 2. Creating and meshing midplane surfaces 3. Using MPC’s (multipoint constraints) to transmit forces in a joint We will be working with the structure shown below. The model consists of 3 plates that are pinned to ground at points A, B, and D, and which are pinned together at point C. The structure supports a load of 40,000 on the plate ABC that is loaded evenly over an area of 20 x 10 (the thickness). We will be using symmetry about the XY plane to reduce the problem size. Material Properties: E=200000; ν=0.3 Figure 1. Isometric View of the Plate Structure Figure 2. Dimensions for Plate Structure ZY1255ABCDXY502050R10R10 (typ)R5 (typ)ABCD1020Step 1: Import the model into Ansys Download the iges file of the part shown above from the course website and save in your CADE directory (home directory or other). Start ANSYS and then do the following: FileÆImportÆIGESÆ(window)leave the default settings and select OKÆ(window) browse to find the iges part where you saved it (the part is called “lab_part.igs”) and open it into ANSYS. Note you can use the mouse buttons to dynamically orient the model if you pick the upper right view menu button (hold cursor over button and it should say “Dynamic Model Mode”). Also, use Plot and PlotCntrls to display the keypoints, lines, and volumes that are automatically brought in with the iges model. Step 2: Modify the model to make use of symmetry WorkplaneÆhighlight the button “Display Working Plane” WorkplaneÆWP Setting…Æ(window) click Grid and Triad. You may want to adjust the size, minimum, and maximum values to 5, 20, and 20, respectively, to help display the working planeÆclick OK. PreprocessorÆModelingÆOperate ÆBooleansÆDivideÆVolume by wrkplaneÆ(window) pick the center plate volumeÆOKÆPartitions the volume down the center into 2 volumes. PreprocessorÆModelingÆDelete ÆVolume and belowÆ (window) pick the volumes forward of the XY plane (i.e. the front plate and the front half of the center plate), then hit OKÆvolumes are deleted. Step 3: Partition the rear vertical plate to create a midsurface (area) WorkplaneÆoffset WP by incrementsÆ(window) type 0,0,-9.5 in the X,Y,Z offsets box and hit OK. PreprocessorÆModelingÆOperate ÆBooleansÆDivideÆVolume by wrkplaneÆ(window) pick the rear vertical plate volume, then hit OKÆPartitions the volume down the center into 2 volumes. Step 4: Select and Display only the areas (midplanes) we will be concerned with SelectÆEntitiesÆ(window) choose Areas and By Num/Pick and then hit OKÆ(window) pick the exposed misdsurface of the center plate and the midsurface of the rear vertical plate which you just created. Plot the areas (or simply type “aplot” in the command prompt); you should see the only the 2 midplanes we are concerned with. Step 5: More Work Plane manipulation and partitioning of the areas for meshing and loading purposes. You may want to look at the figure below as a guide for what the final partitions should look like. WorkplaneÆAlign WP withÆGlobal Cartesian (you may need to replote to see effect).WorkplaneÆoffset WP by incrementsÆ(window) adjust the degrees sensitivity to 90 by sliding button, then hit the +Y button once, and then hit the X- button once. PreprocessorÆModelingÆOperate ÆBooleansÆDivideÆArea by wrkplaneÆ(window) pick the rear vertical plate area, then hit OK. WorkplaneÆoffset WP by incrementsÆ(window) type 0,0,10 in the X,Y,Z offsets box and hit OK. PreprocessorÆModelingÆOperate ÆBooleansÆDivideÆArea by wrkplaneÆ(window) pick the rear vertical plate area, then hit OK. WorkplaneÆoffset WP by incrementsÆ(window) type 0,0,30 in the X,Y,Z offsets box and hit OK. PreprocessorÆModelingÆOperate ÆBooleansÆDivideÆArea by wrkplaneÆ(window) pick the rear vertical plate area, then hit OK. ETC…. Keep partitioning the areas until you have what you see below. Remember that you can always realign the work plane to the global coordinate system in case you loose track of the Work Plane orientation. Figure 3. Partitioned Midplane AreasStep 6: Define Material Properties PreprocessorÆMaterial PropertiesÆMaterial ModelsÆ(window) double click Structural/Linear/Elastic/IsotropicÆ(window) input modulus and Poisson’s ratioÆOKÆ(close Material Model window). Step 7: Define Element Type 1 (for shell elements) PreprocessorÆElement TypeÆAdd/Edit/DeleteÆ(window) Add…Æ(window) highlight Shell63ÆOKÆCLOSE. Step 8: Define Physical Property Set 1 (thickness for shell63 elements) PreprocessorÆRealConstantsÆAdd/Edit/Delete Æ(window) Add…Æ(window with element Shell63 highlighted) OKÆ(window) input thickness of 5 (because we have constant thickness, only the first value is required)ÆOKÆCLOSE. (Note that because we are using symmetry, the middle plate will be the same thickness as the rear plate). Step 9: Select and Display only the lines we will be concerned with SelectÆEntitiesÆ(window) choose Lines and Attached to, then select Areas and hit OKÆ(window) pick the areas on screen or just select Pick All (since we previously filtered our areas to just these midsurfaces) and then hit OK. Step 10: Use the Mesh Tool to set up element divisions on lines and mesh the areas PreprocessorÆMeshingÆMesh Tool Æ(window) under element attributes, set the button to Area, then hit SetÆ(window) select the Pick AllÆ(window) shows material properties, real constant sets, and element type that we are going to be applying to the areas; hit OK. Now the Mesh Tool should still be up (if not just select it again from commands). Use the Set button under the Size Controls, Lines option to assign the element divisions shown in Figure 4 below: Figure 4. Divisions Applied to Lines for Mesh Control 555555555525 25251010101010101010555555555555555555555555555555After you have assigned all the element divisions to the lines, go back to the Mesh Tool and select that you want to mesh Areas, using a Quad shape and Free, then select MeshÆ(window) hit the Pick All button to mesh all the areas. The resulting mesh should look something like this: Figure 5. Mesh of the Plate Midsurfaces Step 11: Define the MPC (Multi-Point Constraint) Element (Type 2) PreprocessorÆElement