Extracting Surface Data at the Centroid

I have created a surface using construction geometry, which creates a cross-sectional cut in my cylindrical geometry I have. I use that surface to create a user-defined plot with the expression set as "Volume" in hopes to calculate the area of each mesh element. However, when trying to extract the results, they all come from a node, rather than the centroid (which doesn't necessarily make sense in terms of area). I have also tried the ECENTX expression and it is still providing values at the nodes. Is there any way to do this yet in scripting?

Find more posts tagged with

IronPython

scripting

Comments

Mike.Thompson

So you want the projected area of a 3D element as cut by a plane?

NikolasYounker

@Mike.Thompson That could possibly work. The purpose of this is to find the 2d bending moments around the principal axis of a plane. I have a macro that does this in ANSYS Classic which utilizes the "sumap" and "suget" command to create arrays of the surface elemental data. So really I need to be able to find the elemental data for both the area and normal stress, if possible. I'm currently using the PlotData.Values as the way to export data from the resulting plots, is there another method I may have missed?

Mike.Thompson

@NikolasYounker ,
If you are looking at bending moments this is = Force x Length from ref point
While you can look at the normal stress (F/A) and multiply by area to get back to force, a more direct route is simply to use the element nodal forces directly without the need to convert to stress and back again.

In Mechanical you can use a moment reaction probe and scope to the construction surface to get the moments per a user-defined local CS.

In APDL you can also use the FSUM command after using ESEL commands to do a split of the mesh.

In PyDPF and/or DPF in mechanical you can also post process element nodal forces and after also looking at nodal locations calculate bending moments.

Does this make sense?

One other option that is more round about is you can take the normal stress and export it. This will likely be at the nodal locations as you mentioned, but in general this will be an accurate field per those locations. You can then use this as external data and create a dummy imported pressure load based on this field on a dummy CAD 2D surface. This pressure will be applied to the 2D elements and you can see the element area and mapped pressure value.
I don't really recommend this option, but if you want a solution that is based on normal stress and doesn't require scripting this would be a way.

NikolasYounker

@Mike.Thompson We never even thought to use the moment reaction probe, thank you for informing me! I think that is all I needed as finding the local bending stresses shouldn't be an issue. Thank you for your help!