Fixing one end and applying tensile load on the other

[ay8tb]

Hi,
I'm trying to compare my results with ANSYS workbench (same model properties, loading and boundary conditions) but I'm getting slightly different results, mainly at the boundary conditions and loading area. I'm fixing one end by the face in workbench and applying tension on the other face. Is this the way to do it? Or am I missing something?

mapdl.nsel("S", "LOC", "Y", 152.4)
        selected_nodes = mapdl.mesh.nnum
        mapdl.d("ALL", "ALL")
        mapdl.allsel()
        selected_nodes = mapdl.mesh.nnum

        mapdl.nsel("S", "LOC", "Y", 0)

        # Check if any nodes are selected at the specified location
        selected_nodes = mapdl.mesh.nnum

        # Next, couple the DOF for these nodes.  This lets us provide a force
        # to one node that will be spread throughout all nodes in this coupled
        # set.
        mapdl.cp(5, "UY", "ALL")

        # Select a single node in this set and apply a force to it
        # We use "R" to re-select from the current node group
        mapdl.nsel("R", "LOC", "X", half_width)  # selects more than one
        selected_nodes = mapdl.mesh.nnum
        # print(selected_nodes)
        single_node = mapdl.mesh.nnum[0]
        mapdl.nsel("S", "NODE", vmin=single_node, vmax=single_node)
        mapdl.f("ALL", "FY", -5700)

        # finally, be sure to select all nodes again to solve the entire solution
        mapdl.allsel(mute=True)

[mikerife]

@ay8tb this probably does not match the FEM in WB Mechanical. The use of CPs in WB Mechanical is pretty rare. Can you show a picture of the applied load in WB Mech? Mike

[ay8tb]

Hi @mikerife, this is how the loading like in WB Mechanical:

With the other end being fixed:

[mikerife]

Hi @ay8tb Ok Mechanical is using a surface effect element and is applying a equivalent pressure to the face with the applied force. Instead of using a couple try this:

mapdl.nsel("S", "LOC", "Y", 0)
selected_nodes = mapdl.mesh.nnum
mapdl.f('all', 'fy', -5700/len(selected_nodes))
mapdl.allsel()

Now how do the results match? Oh, and compare with linear elements to start.

[ay8tb]

Hi @mikerife, I replaced that and it looks like the von Mises stress doubled at a couple nodes, when compared to the WB:

[mikerife]

@ay8tb looks good; apply St Venants principal. How do the results compare now?

If you want the results to match closer, then create the surface effect elements in PyMAPDL and apply the appropriate pressure.

[ay8tb]

Hi @mikerife, I'm a little confused on how to apply this, is there any documentation I can refer to?

[ay8tb]

Hi @mikerife any additional information I can provide? Is there any documentation on how I can apply St Venants principal in PyMAPDL?

[mikerife]

Hi @ay8tb
For anyone not familiar with St Venant's Principal see here.

@ay8tb you could just unselect the first set of elements one element into the volume from the surface with the applied load. Or maybe the first two.

Here is an example of using coupling, directly applied force, and applied pressure. 2-3 elements away from applied load the stress fields are identical. So the question is how accurate of a result do you need at the region of applied load. If very accurate, then we need to be more accurate in our method of 'recreating reality' with the load.

Mike
3334.zip

[germa89]

@ay8tb you can always compare your PyMAPDL code with the ds.dat file exported by Workbench.

Converting the ds.dat to PyMAPDL code (using the converter for instance) should give you the very same model in PyMAPDL as the Workbench one.

Having both codes allows you to compare.

I believe exporting the ds.dat file is an option in Workbench Solution tab, but probably @mikerife, @mcMunich or @pmaroneh can let you know for sure.