Learning Forum

[Francisco Sousa]

On Mechanical, I am doing a Static Structural simulation using SOLID185 elements and i want to obtain the Stress (Cauchy) Tensor values in the Integration (Gauss) Points, and the Integration Point Coordinates.
Using Command Blocks, I used the ERESX,NO command, wich gave me the values of the equivalent stress in the gauss points, associated with the closest node. I attempted to use the PRESOL,LOCI and OUTRES command, but Ansys does not allow them to be used with this type of element. I also attempted to use ESOL and KEYOPT commands, but was unable to (I am unsure how to write these correctly).

How can I obtain what I need? Must I use Mechanical APDL and not Mechanical with Command Blocks? Is this a syntax problem? How can I find the correct syntax rules?
Thanks in advance.

[Mike Rife]

Hi Francisco

The integration point locations are available for Solid185 but large deflection needs to be turned on (in Analysis Settings).  Also they (integration points) need to be stored to the results file, but it's not an often needed quantity so a environment commands object needs to be used to turn on saving them to the result file.  In the commands object use the command:

outres,loci,all

This commands object is not the one used to post-process them (presol,loci).  You should also look up the /outp command in the Mechanical APDL help as you probably (not sure) want to redirect the integration point listing to a separate file...or maybe not.

Mike

[Francisco Sousa]

Thank you for your reponse!
Is it possible to obtain the values of the stress tensors in the integration points, as well as their coordinates, together? That is, a file where the Integration points are listed, as well as their coordinates and their stress tensor values.

[Mike Rife]

Hi Francisco

Well...like one command to dump all of that at once to a file?  No.  We need to gather the data then write the data to a file.  Integration point locations can only be printed out from MAPDL.

Now an interesting point is that the PyMAPDL Reader can access the integration point locations in the result file if written.  See https://reader.docs.pyansys.com/user_guide/loading_results.html (seach for the word integration).  The PyMAPDL Reader is just that, is reads a MAPDL result file and is part of the open source PyAnsys project.  Since it is a reader and there is no instance of MAPDL that it is interacting with many controls that MAPDL users are used to are missing i.e. selection logic.  However it does recognize MAPDL components.  You would still need to gather then write to a file the locations.

The PyMAPDL Reader is being deprecated and replaced by PyDPF but I don't see in its documentation that we can get the integration point locations.  Keep in mind it is a) very new and b) being actively/rapidly developed so this may change soon.  Or you could add open an Issue for it to have the functionality added.  https://dpf.docs.pyansys.com/version/stable/getting_started/index.html