Mirror a named selection of selected faces in Mechanical Workbench

I have a semi-symmetrical model and it has a cluster of facets.


I have a named selection of a group of selected faces on one side of the model and I want to reflect this selection to the other side of the model.


I am looking to mirror the selection itself and not the faces, as the faces already exist on the other side of the model.


It's pretty inconvenient to select these groups of identical faces manually on each side of the model due to the dense cluster of facets.

Best Answer

Answers

  • You can't mirror an existing selection that was created by picking individual faces.

    If you had made the original selection by using the Worksheet and coordinates, you could have added another row and simply changed the sign on one of the coordinates.

  • Unfortunately, the original selection can't be created using a worksheet due to the complexity of the geometry surface.

    I have to select these facets one by one in groups. And once the selection is done, I can't edit its coordinates.

    Then I have to figure out a way to reflect this selection to the other side of the model.

    It seems the only way is to select these facets individually on each side considering obtaining an identical end result on both sides.

  • AniketAniket Forum Coordinator

    Or you can use ACT to loop over selection, calculate centroid of the faces, and loop over all the faces and find faces that matches centroids in existing named selection within a tolerance.

    If your model is perfectly symmetric, I would rather suppress the other half of the model and use Model assembly to mirror it.

    -Aniket

    How to access Ansys help links

    Guidelines for Posting on Ansys Learning Forum

  • Ahmed_5AAhmed_5A Member
    edited September 22

    I think this could be achievable by the following:

    -Convert selected facets to vertex -or mesh node- in worksheet selection

    -export vertices coordinates (I couldn't find an option to do that, it's possible only to export mesh nodal ID CDB file and nodal coordinates as a txt file, is there a way to do the same with vertices?)

    -edit one of the coordinates of the vertices

    -import the edited file (like importing selections from CDB file)

    -Convert vertices cloud into faces again using worksheet selection 

  • AniketAniket Forum Coordinator

    Ahmed_5A, I honestly believe this would be a very tedious way to do this. but if you prefer it you can give it a try and let us know!

    Also to answer, you can select anything in the GUI vertices or nodes, you can go to selection information and can export it to text file from the selection manager window.

    But for step one in your algorithm, if you are already converting manually selected named selections to worksheet based one, as peter said, you can simply duplicate and change sign of the one coordinate there, would do the trick!

    -Aniket

    How to access Ansys help links

    Guidelines for Posting on Ansys Learning Forum

  • I couldn't find an option to export selected vertices to a text file from the selection manager window!

    As I mentioned earlier this option of export and import is available only for nodes, not vertices!

    Concerning step one in the algorithm, I select faces on one side, then I convert it to vertices using worksheet selection as shown in the attached image, but I don't get any access to the coordinates of these vertices in the worksheet to edit it, is there a way to do that?

  • AniketAniket Forum Coordinator

    Ansys staff can not download images on the student portal, so if you want to reach a larger audience to get answers from, please insert the images inline.

    Also, I was referring to "Selection information" tool:


    Also, Have you done the following steps manually:

    -import the edited file (like importing selections from CDB file)

    -Convert vertices cloud into faces again using worksheet selection

    I am not sure if those are doable in Mechanical without doing scripting.


    Best bet would be using Model assembly (https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_mesh_mod_alignment.html) with half model and then simply mirror the entire mesh and assemble it. (Assuming the model is split at symmetry plane)

    Next best to defining them manually would be using ACT as I mentioned in previous post to create them programmatically.

    -Aniket

    How to access Ansys help links

    Guidelines for Posting on Ansys Learning Forum

  • Yes, I did the following manually:

    -Exporting selection as txt file and CDB file

    -Find the mirrored nodes ID and create a CDB file of the mirrored nodes

    -import the mirrored nodes CDB file

    -Convert nodes cloud into faces again using worksheet selection, and here I have an issue:

    the feature works but the regenerated facets selection includes also the bordering facets of the nodes,

    what I target is the facets enclosed only by these nodes,

    it seems the algorithm of Workbench includes all of the faces which have intersecting node with the cloud of nodes.

    is there a way to dismiss these bordering facets from the regenerated selection?

    (again I see that you use vertices not nodes in your feedback replies despite they are totally different -vertices are a geometry property where facets mate, while nodes are a mesh dependant-, the only option I find is exporting and importing mesh nodes ID and XYZ as CDB and txt files respectively, is there a way to do the same with vertices?)

    I apprecite your feedback.

  • AniketAniket Forum Coordinator

    is there a way to dismiss these bordering facets from the regenerated selection?

    You can try the following:

    have edge nodes subtracted from the set, first create a named selection for edges, then convert it to nodal, and use worksheet to subtract it from your existing nodal named selection for the face. But again this would work only if your original model has the edges.

    -Aniket

    How to access Ansys help links

    Guidelines for Posting on Ansys Learning Forum

This discussion has been closed.