mesh_skin operator in Mechanical DPF extracts contact elements – area doubled

Hello everyone,

I’m using Ansys Mechanical 2024 R2 and want to calculate the surface area of my mesh via the mesh_skin operator within an ACT Application. However, the resulting mesh_skin includes additional elements (probably due to the contact elements), which leads to double the expected area.

Here is my code:

skin_mesh = dpf.operators.mesh.skin(
    mesh=full_mesh,
    mesh_scoping=node_scoping
).outputs.mesh.GetData()
area_field = dpf.operators.geo.surface_area(mesh=skin_mesh).outputs.fields_container.GetData()[0]

In node_scoping are all nodes on the area (which is the geometry of interest).

The skin_mesh.ElementCount indicates double the element_faces which should be there. This causes me problems by calculating the area of the element faces and I need the area_field because I do additional calculations with this field and a stress field but the length doesn't match.

Is there a way to get the skin_mesh just for the solid elements?

Regards
Felix

Find more posts tagged with

Mechanical

DPF

Accepted answers

fkaule

Hello,

the solution was to get the mesh just from solid elements:

solid_op = dpf.operators.scoping.on_mesh_property()
solid_op.inputs.property_name.Connect("solid_elements")
solid_op.inputs.mesh.Connect(full_mesh)

scoping_solids = dpf.operators.mesh.from_scoping()
scoping_solids.inputs.mesh.Connect(full_mesh)
scoping_solids.inputs.scoping.Connect(solid_op)

skin_mesh_op = dpf.operators.mesh.skin()
skin_mesh_op.inputs.mesh.Connect(scoping_solids)
skin_mesh_op.inputs.mesh_scoping.Connect(scoped_nodes)
skin_mesh = skin_mesh_op.outputs.getmesh()

Regards
Felix

All comments

James Derrick

Hey @fkaule that's a great question. I've pinged the @Structures-Scripting-Team and hopefully one of them will be able to help.

Mike.Thompson

@fkaule ,
I would not have expected this behavior due to the contact, but I do understand your hypothesis and it makes sense.

The "skin" operator takes in 2 key inputs that are similar, but do have different purposes.
1. The mesh
2. the mesh scoping

The mesh is the base mesh you are working with and I think the solution to your issue. If you only want to skin overlay on the solids, then the mesh input should only have the solids. There are a number of ways to get the mesh with only the solids.

One way is to use: op = dpf.operators.mesh.from_scoping() # operator instantiation
Or a similar operator: op = dpf.operators.mesh.mesh_extraction() # operator instantiation

Both of these extract a subset of the starting mesh and could be used to filter out any contact or non-solid elements from the mesh. So in the initial step you have a mesh scoping that is elemental and ONLY contains the solid elements of interest.

You then pass this mesh object to the skin operator and the contact elements that are causing your troubles are not in the mesh, and you use you nodal mesh scoping as-is in the skin operator.

In the end you have an elemental mesh scoping to reduce the mesh, that is then passed to the skin operator with a 2nd mesh scoping (that is nodal).

fkaule

Hello,

the solution was to get the mesh just from solid elements:

solid_op = dpf.operators.scoping.on_mesh_property()
solid_op.inputs.property_name.Connect("solid_elements")
solid_op.inputs.mesh.Connect(full_mesh)

scoping_solids = dpf.operators.mesh.from_scoping()
scoping_solids.inputs.mesh.Connect(full_mesh)
scoping_solids.inputs.scoping.Connect(solid_op)

skin_mesh_op = dpf.operators.mesh.skin()
skin_mesh_op.inputs.mesh.Connect(scoping_solids)
skin_mesh_op.inputs.mesh_scoping.Connect(scoped_nodes)
skin_mesh = skin_mesh_op.outputs.getmesh()

Regards
Felix