How can I extract mesh data from a selected face / body?

Nikos Kallitsis
Nikos Kallitsis Member, Employee Posts: 36
10 Comments 5 Likes First Anniversary Ansys Employee
✭✭✭✭
in Structures

I have selected a face / body and know the ID of the item. How can I retrieve some mesh information like elements and nodes?

Tagged:

Best Answer

  • Nikos Kallitsis
    Nikos Kallitsis Member, Employee Posts: 36
    10 Comments 5 Likes First Anniversary Ansys Employee
    ✭✭✭✭
    Answer ✓

    This can be achieved with some Python commands executed in the Mechanical Scripting interface.

    First let's check how you can get the face / body Id. Assuming you've created a Named Selection scoped to the face(s) / body(ies), you can select that object and check the Ids of the scoped parts:

    sel = DataModel.GetObjectsByName('NamedSelection')[0]
selectionIds = sel.Ids

    To get the element / node data, the mesh associated with the selected face / body must first be selected. In the case of a face with Id = 7 for example:

    myFaceId = 7
meshData = ExtAPI.DataModel.Project.Model.Analyses[0].MeshData
meshFace = meshData.MeshRegionById(myFaceId)

    Then the element / node data can be retrieved from the meshFace object:

    elementIdsMeshFace = meshFace.ElementIds
elementIds = meshFace.ElementIds
nodeIds = meshFace.NodeIds

    To access the element / node objects themselves:

    elements = meshFace.Elements
nodes = meshFace.Nodes

    To retrieve the X, Y, Z, coordinates of a selected node:

    xLoc = nodes[0].X
yLoc = nodes[0].Y
zLoc = nodes[0].Z

    In the case of bodies, the commands are exactly the same.
    To export the desired data to a text file, you can do so by using the usual Python commands with the 'os' library after importing it.

Categories