Plotting Results on a subset of Volumes

[AidanMcConneheyOVT]

Hi everyone,

I'm working on setting up an automated PyMAPDL script, but I am curious what the best way to export a result on a subset of bodies is.

For instance, I have a multibody/material assembly with a conformal mesh, but the stress is all concentrated around specific parts that I would like to plot individually.

Any tips or methodologies for this would be greatly appreciated!

[mikerife]

Hi @AidanMcConneheyOVT
Please see the MAPDL Command Help Guide on the selection commands. There are two types of select commands. The first has the form xSEL where x is a letter representing what you want to select. So NSEL is Node SELection. VSEL would be Volume Selection. The second type of selection command is a 'select x of y' type of command where the form is xSLy. So ESLA would select the elements associated with the current set of meshed areas.

Selections have a lot of criteria depending on what is being selected. We can select elements based on their properties like assigned TYPE or 'Element Name' of the assigned type, assigned material ID, applied load value....etc. Nodes can be selected by result quantity, position, etc.

Given all that any tip would depend on what you actually want to post process. For example say you want to just see the region where X stress is greater than 1000. Then this could be used (but not the only way!):

mapdl.nsel('s', 's', 'x', 1000, 1e8)
mapdl.esln('s')
mapdl.nsle('s', 'all')
mapdl.post_processing.plot_nodal_component_stress('x')

Or take your example, if the specific parts are three parts with material IDs of 4, 5, 6 assigned to their elements we could do:

for matid in range(4, 7):
    mapdl.esel('s', 'mat', '', matid)
    mapdl.nsle('s', 'all')
    mapdl.post_processing.plot_nodal_eqv_stress()
mapdl.allsel()

Let me know if you run into any questions/issues or have a specific example in mind.
Mike

[AidanMcConneheyOVT]

Hi Mike, thank you that's very helpful. I had no idea the plot_nodal_solution() methods responded to the active selection.

Going a bit farther, I am hoping to utilize built in PyVista methods for post processing, as outlined here: (https://mapdl.docs.pyansys.com/version/0.68/examples/gallery_examples/00-mapdl-examples/path_operations.html#sphx-glr-examples-gallery-examples-00-mapdl-examples-path-operations-py)

Hopefully this will allow an increased ability to automate things like reports and output data.

Do you know how I could go about selecting all elements/bodies with a specific material, and then only plot these utilizing the PyVista implementation?

[mikerife]

Hi @AidanMcConneheyOVT
See the PyMAPDL mesh.grid method. This will create an PyVista data object (I think that the right term) of the selected mesh. From there you gather some result and use PyVista to plot. So given your description, say the important mesh has material ID 3:

.... stuff to build solve model etc.
import pyvista as pv
mapdl.post1()
mapdl.set('last')
mapdl.upcoord(1)
mapdl.esel('s', 'mat', '', 3)
mapdl.nsle('s')
mesh = mapdl.mesh.grid
result = mapdl.post_processing.nodal_component_stress('x')
mapdl.allsel()
mapdl.upcoord(-1)

plot = pv.Plotter()
plot.add_mesh(mesh, scalars=result, cmap='jet')
plot.add_title("X Stress of Material 3")
plot.show()

The upcoord add the nodes deformations to their positions so we get a deformed mesh to show instead of the original geometry.

Mike

[AidanMcConneheyOVT]

Hi Mike,

That works great, thank you for the help!