How do I make/prepare an ANSYS mesh for import into CFX Pre?
**************************************************************
|
If you have an ANSYS db file already you can convert it to a cdb file in ANSYS by: 1. Opening the ANSYS database in ANSYS. 2. Issuing the ALLSEL command to select everything. 3. Issuing the CDWRITE,DB command to write the cdb file. To get a list of all element types (ET)/keyops(KEYOP) that are supported by mesh import, you can run the following from the operating system command line: <CFXROOT>/bin/<OS>/ImportANSYS.exe -S Note: Before executing the CDWRITE command, verify that the data base has a separate named component of 2D MESH200 elements for each surface that will require a boundary condition. Delete any MESH200 elements that are not members of named components. To define specific 3D regions, create a 3D named component of 3D elements. The component names will appear in CFX-Pre as defined regions. ************************************************************* If creating your ANSYS Classic mesh from scratch, you must use an appropriate element type. Its best to try to use a 3D structural element like Solid45, or perhaps Fluid142. Once you have your mesh, you need to define nodal component groups to representyour boundary locations. The quickest way to do this is to type 'asel,s,p' and then pick a surface(s) for the location. When done, type 'nsla,s,1' to select all nodes associated with that surface. Then type 'cm,locname,node' changing the locname as appropriate, to create the group. Repeat for all locations, and then finish by typing 'allsel'. Export the file by typing 'cdwrite,db,myfilename,cdb' chaning the filename as required. When importing the mesh into CFX-Pre, select the ANSYS filter and the .cdb file you wrote out. You may get a message about midside nodes being ignored but that is perfectly normal especially if the file has come from Workbench. ****************** |
||
|