How do I get information about the total volume or area

[Deternanna]

Hi!
Maybe this seems like a simple question, but I cannot seem to find the answer anywhere.

I have created a geometry in Python, using the ansys mapdl package. The geometry is made of rectangular beam elements (1x1 mm). Is there a smart way for me to get the information on the total area/volume of the full geometry (of all elements)?  ( I have attached a photo of the geometry). Hope you can help!

[mikerife]

Hi @Deternanna so first, please be careful with the terminology as beams are not geometry in MAPDL. So when you say you created the geometry do you really have keypoints and lines, which were then meshed? Or did you create nodes and elements directly? Some combination?

If there are lines you can use LSUM to calculate the total length of the selected lines. Then *GET (PyMAPDL get_value) to retrieve that sum.

Length is not an property of a beam element that can be retrieved, but it can be calculated. If only the FEM exists then we can loop over the beam elements and calculate the length from the node positions. Unfortunately PyMAPDL Queries does not include the 'distnd' APDL short cut so you'll need to create your own function. Pretty straight forward with the nx, ny, nz queries using get to get the i and j nodes of the element.

Mike

[mikerife]

Hi @Deternanna sure, see the MAPDL help on the *GET command, in the Solution Items section. We can retrieve the total mass and other related properties after either an 'normal' solution that involves mass or as you are showing after an inertial relief calculation. Just use the PyMAPDL get_value to retrieve it to a Python variable.

Since this mass is coming directly from the mass matrix it's also a good check of the mesh. If the CAD mass and the FEM mass don't agree, then maybe the mesh is too coarse. Or something.

[Deternanna]

Hi again Mike,
I feel like I have tried that already, but the syntax just doesn't seem to include the mass. And as you say, I can't get the volume in this way, because I have only created the FEM elements.

I have tried running these in the solutions item section:

mapdl.get_value(entity = 'TOTAL MASS')
mapdl.get_value(entity = 'MASS')
mapdl.get_value('TOTAL MASS')
mapdl.get_value('MASS')

[Deternanna]

Hi Mike,
I followed up with the suggestion you had of making a loop over the beam elements and calculating the length from that. And that solution is now working. I am still very interested in getting out the mass property as a Python variable, because when I start making elements with varying cross-sections, it will get very hard to keep track of which elements have which cross-sections. I plan to keep the density the same, so this would provide me with a variable that can generate the volume in the correct way every time.

[mikerife]

Hi @Deternanna
Well, the 'Entity' is not 'Total Mass'. It is 'elem'. The Item is total mass (MTOT) and item number the direction (i,e, X). So to get the total mass the command would be:

total_mass = mapdl.get_value('elem', 0, 'mtot', 'x')

And we can get the element volume with some caveats. For example the volume is that defined by the nodes defining the element connectivity. For (linear) beam elements there are only 2 nodes...so we can get the length of the element with *get. From there we can *get the section number 'attibute' of the beam element. Then *get the area of the cross section from the section properties for that specific section number. Combine the two and we have the volume.

The process is 'easier' for a 3D element since its node connectivity defines a volume, which can be retrieved with *get.

Mike

[Deternanna]

Hi Mike,
Thank you so much - this was exactly what I was looking for!