Nan error while reading rst ansys result file

[swatz3221]

Hello,
I am new to python and I tried using pyasnys library to read an .rst ansys result file. I was able to read all the displacements at each node but was not able read read the stress values and strain value after a certain nodes. It showed up Nan error after few nodes. Can anyone suggest me to read all the values without a Nan error? I am attaching the screenshot also for clear understanding.

[pmaroneh]

Hello,
My two cents here. Could it be that the nodes that return a NaN value are not standard mesh nodes, and so would not have a stress/strain value ? I'm thinking beam orientation nodes, or contact nodes, etc.
Another possibility might be that the output settings were set in such a way that the stress/strain values were retained for some regions of the mesh only (specific named selections).
Please note that mapdl.reader is legacy, I would suggest that you try using DPF (Core or Post) for opening and post-processing of an .rst file.

[RGPATCHI]

Hello @swatz3221,

Just an addition to what @pmaroneh has suggested, please note that the rst doesn't have stresses stored at mid-side nodes. So, please check if the node numbers for which stresses are NAN, are indeed midside nodes.

I just tested a simple example with Solid186 (i.e. with mid side nodes) and Beam188 (with Orientation nodes) and as expected, I get NAN at both Midside and Beam orientation nodes.

Hope this clarifies. And I would suggest using DPF as well, as reader is legacy and with DPF, we can get the stresses at midside nodes as well (calculated on the fly from the corner nodes).

Best regards,
Rohith

[akaszynski]

Agreed regarding DPF, and this is another reminder for us to switch our example documentation over to using DPF.

Pinging @rlagha for visibility.