Assigning element type in ANSYS Workbench 3

[rupika]

Hi all,
I want to assign element type in ANSYS Workbench. But I couldn't find any method for that. Could anyone help me? I am struggling to do it therefore your help is great appreciated.
Thank you very much.

 

[Maud35]

http://www.eng-tips.com/viewthread.cfm?qid=232126

does it help ?

 

[rupika]

Thank you for the link. I want to know that how to assign BEAM189 element and SHELL element in workbench.

 

[Maud35]

you create a line body, and RMB on "mesh" -> "method" -> "element midside nodes" : you choose "kept" to get a "beam189", "dropped" for "beam188".
and to get shell element, you create a surface and mesh it?

 

[TQFP]

1)you need to create a command windows
2)you can use ET,, command, it should be: ET,1,BEAM189

 

[rupika]

Thank you very much for the reply. I opened command window in engineering data file. Then I wrote ET,1,BEAM189 command but when I enter it the following error message is appearing.
UnboundNameException: name 'ET' is not defined
I am new to ANSYS workbench so I have confused. Should I introduce ET in first lines in the command window? Could you please explain it for me? Sorry for disturbing.

 

[Calcul8it]

Take a look at my answer here:

http://eng-tips.com/viewthread.cfm?qid=319224

For the element type number you should not write, say Beam189, but write: et, 1, 189

You write it in Mechanical by right-clicking on each body (that you want to change element type for) and click Command/add comment (can't remember precisely) and paste the above in the window that appears.

Not sure if you can directly force elements to have midside nodes in Workbench just by adding this command on each body, you might have to mesh first, with option "midside nodes kept", in order to get degenerate/midside noded elements. If you run into troubles I would suggest you to convert all the Beam188 to Beam189 in Ansys classic, i.e after export from Workbench.

Good luck!

Christian Hansen

FEA consulting made easy -

http://www.calcul8.it

 

[rupika]

Thank you very much all for your great help.

 

[ru263]

I opened Mechanical and right-clicked on the body that you want to assign element type for. But I couldn't find Command/add comment from that. I have attached what I could find after write clicking on the element body. Still I am struggling to assign element type in workbench. Please help me!!

 

[Calcul8it]

Hi ru263

Looked at your attached screen-dump from Ansys Mechanical - and you're close to the right place!

Look at the section on the left side of the screen (I think Ansys names this space something like "Project Outline"), click on the "+" where there is a question mark and the word Geometry "? Geometry" - now you see the list of bodies in your geometry (it looks like you only have one body in your geometry). Right-click on the body you wish to change default element type for and now, in the drop-down menu you should have the option of adding command/comment.

When you click 'add command' you are shown a white space, where you can paste in
"et, matid, 186" (Solid186 or whatever solid element type you need). Unfortunately you have to do this on each body you want to change (but now you have just one body , and if you change the fundamentals of the geometry in DesignModeler (say by merging/joining/union this body with another), then I think the add command will be lost next time you come to Mechanical because this is then essentially a new body (just check the command when you have changed the geometry).

If I remember correct, these added commands will be executed just prior to execution of the solve command, if you solve directly in Workbench Mechanical. If instead you export the mesh (Click "Static Structural" in "Project Outline" -> "Tools" -> "Export ... ") the command will be executed as the mesh file is generated so that the mesh file contains your desired element type.

I find Workbench somewhat unpredictable, so if you want to be sure exactly what happens when, I suggest you do your modeling and meshing in Workbench and then export the mesh (and loads/constraints if those are applied in Workbench) and read-in the exported .inp file i Ansys Classic (.inp is the same syntax as .cdb but for some reason Ansys changed it in the export tool). In Ansys Classic you can easily change element type and actually inspect the elements to see things are performed as you expect.

Good luck!

Christian Hansen
Twitter: @chrhansen


FEA consulting made easy -

http://www.calcul8.it