Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

ANSYS Workbench and MESH200 Elements: EMODIF

  1. Jan 24, 2016 #1
    Hello all,

    I have been doing a number of analysis that require the use of Workbench and Spaclaim and Classic (APDL).

    SpaceClaim is used to bring in the geometry and defeature it and to create the proper components with elimination of contacts thru the use of the Share Topology feature. This is a huge time saver and eliminates the use of the clunky old (not updated for over 20+ years) classic APDL geometry editor and the defeaturing tools are excellent and very easy to use.

    Workbench is used to set the material properties and create the mesh. Meshing in Workbench on complex geometries is highly efficient. However, the amount of control over the mesh in Workbench isn't as great as it is in Classic. I prefer to used older elements, some of which are classified as Legacy, and Workbench isn't going to select a SOLID45 for a Static Structural mesh. So what does one do? EMODIF is the answer.

    To get from Workbench to Classic APDL you can:

    1. Insert a Command snippet that issues a simple SAVE,FILENAME,DB and then browse to the correct folder located inside of the Workbench file structure

    2. Create an ANSYS component in the Workbench Project page and go over to Classic APDL using the "EDIT IN ..." command by right clicking in the proper place.

    Now once in Classic APDL all the model consists of is nodes and elements. The elements are all null type MESH200. A solution cannot be run on these elements as they are just place holders.

    First, create the element types that are needed for the solution. For example, SOLID45 for a stress solution. Now, SOLID45 elements have midside nodes that are not wanted and if they haven't been dropped (this is done over in Workbench before bringing the mesh into Classic APDL) the MESH200 elements will consists of 10 nodes instead of the desired 8 nodes. (As a general note: never use midside nodes.)

    !!Create the element types
    ET,10,45

    This states that element type number 10 is SOILD45 (The 10 is arbitrary)

    !!Select all the element types that make up the component
    ESEL,S,TYPE,1,2,1

    This states the element types 1 and 2 are to be selected and these numbers would have to be tailored to your model. To get a listing of all of the types issue the ETLIST command.

    Once selected, issue the EMODIF command

    EMODIF,ALL,TYPE,10

    And now the component consists of SOLID45 elements. If a warning is displayed about shape checking that means the nodes do no match up and the MESH200 elements have different number of nodes then the elements that are trying to change them to. Correct this until no warning message is displayed.

    EMODIF will work for a number of different items. For example, material properties can be applied to elements in the same manner. Select the desired elements and issue EMODIF,ALL,MAT,1 (again the 1 is arbitrary).
     
  2. jcsd
  3. Jan 29, 2016 #2
    Thanks for the post! This is an automated courtesy bump. Sorry you aren't generating responses at the moment. Do you have any further information, come to any new conclusions or is it possible to reword the post?
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: ANSYS Workbench and MESH200 Elements: EMODIF
Loading...