Femap_四面体单元网格质量

Distortion in Tetrahedral Elements1.If you have not done it already, you should download the file Tee.x_t from the a link on the MAE-5020 webpage. In FEMAP use the menus File/Import/Geometry to read in this Parasolid file. Parasolid files are store in units of meters. To get units of millimeters we need to enter a Geometry Scale Factor of 1000 as shown below before clicking OK to import the Parasolid file. You should now have the image shown below.2.Restrain all translations on the positive Z surface as shown below. Use the menusModel/Constraint/Surface to do this. You and just click OK on the first popup window for a constraint set name. In the next “Entity Selection” window select the surface shown below and click OK. In the “Create Constraints on Geometry” window, select the Pined radio button. Click OK and Cancel.3.Apply a 1000 mN/mm2 pressure on the positive X surface as shown below. Use the menusModel/Load/Surface, key in a Load Set name, select the surface and click OK, and in the popup window shown below, select Pressure and enter the pressure value. Click OK and Cancel.4.We will next set the mesh control to make a coarse mesh. From the menus select Mesh/Mesh Control/Sizeon Solids. Select the solid and click OK. In the popup window, make sure Tet Meshing is selected and key in an Element Size of 35. Click OK.5.Next, mesh the part by using the menus Mesh/Geometry/Solids. Since we have yet to define a material, thewindow below pops up. Key in the values shown which a representative for steel and click OK. In the Automesh Solids popup window you can just click OK using the default SOLID Property.6.You should now have the mesh shown below. We will turn off the solid to more clearly see the mesh. Aneasy way to do this is by clicking the icon. This toggles the geometry on and off.7.Notice that the edges of each tetrahedral element are straight. This is the default approach used by FEMAP.This overly coarse mesh does not well represent the geometry because of the straight edges. However, ifcurved edges were used, it creates elements with much more distortion (sufficient that an analysis couldfail). Let’s examine the distortion in the elements in this model. Select from the menusTools/Check/Element Quality. In the first popup window, click the Select All button to select all theelements and click OK. In the Check Element Distortions window, only select Aspect Ratio and Jacobian to be checked as shown below. This will make a list of elements with either Aspect ratios greater than 12 orJacobians greater than 0.85 to be displayed. We are also asking to create a group containing these elements.Click OK. A small portion of the display in the Messages window is shown below.Element Aspect Ratio Taper Alternate Taper Internal Angles Warping Nastran Warp Tet Collapse Jacobian Combined405 2.17881 0.86823 418 2.32891 0.85428 453 12.6647 0.66574 479 12.014 0.662248.The following information is from FEMAP’s documentation:“Valid elements prod uce Jacobian Distortion values between 0.0 and 1.0, where 0.0represents the "ideally shaped" element. Severely distorted elements whose Jacobiandeterminants are locally discontinuous or undefined are assigned a distortion value of 2. Ifany of your elements have a Jacobian Value of "2", the element is not valid (i.e., theelement is inside out, twisted, etc.) and should be fixed before analysis.”Thus, what FEMAP calls a Jacobian is not the same as the determinate of the Jacobian matrix as described in your text. However, per their guidelines, a 0 for distortion would be a perfectly shaped element and a 1.0 is on the outer limits of acceptance. If a value of 2.0 is obtained, the element is invalid! If you look through the message window, the worst distortion is 0.87346. Not a great element, but it will solve.To look at the elements in the group that was created, go to the Model Info window as shown below and click on the + in front of Groups, then right click on the group named “Distorted Elements” a nd selective Activate. Right click again on the group name and select “Show Active Group.”9.Your display will look something like the one below. If you rotate the model around, you will see theelements are getting very flat. Automatic meshing of tetrahedral elements can produce “flat” elements (i.e.they have very little volume).10.To displa y all the model instead of these “bad” elements, right click on the group name again and select“Show Full Model” as illustrated below.11.Proceed with a normal static solution as you have done before. You should not get any error messages.12.Click the icon and set the Contour parameter to Von Mises Stress and click OK. Click the andicons to display the deformed stress results.13.We will delete the results and the model. In the Model Info window, expand the Results + and right click onthe case and select Delete as shown below. In the next popup window, click the Go Fast button to delete the results.14.Now from the menus select Delete/Model/Mesh. In the popup window click the Select All button. In thenext popup window it asks if you want to delete unused properties and materials. Click NO.15. Because we turned off the geometry display, the screen looks funny. We need to turn the geometry backon. An easy way to do this is by clicking the icon.16.We will now mesh with more nodes. Select from the menus Mesh/Mesh Control/Size on Solid and selectthe part and click OK. In the popup window enter an Element Size of 10 and click OK.17.Next create a mesh on the part using the menus Mesh/Geometry/Solid. After making the mesh, your displayshould look like the one below. Notice how the mesh now more closely follows the curved geometry.18.Check the distortion in the elements again using the same parameters as used before. You will find that theJacobian values are reduced somewhat (0.873 to 0.786) but the aspect ratio has increased in some cases.You will find these elements located in corners of the joints and some mesh refinement in those areas might further reduce the aspect ratios.19.Look at the “worst” elements in the group we just created. In the Model Info window right click on thesecond group name to “Activate” and then “Show Active Group.” You will find these elements located in corners of the joints and some mesh refinement in those areas might further reduce the aspect ratios.20.Redisplay all the model by right clicking again on the second group name and selecting the “Show FullModel” item again. Next, solve this model. Display the Von Mises stress contour on the undeformedbody . Turn off the geometry display by click the icon. Turn off the nodes using the icon.When you have a fine mesh it helps to turn off the element edges. You can do this by holding down the left mouse button on the icon shown below and selecting the Filled Edges icon. Print this out and hand it in.。