Is it possible to automatically read Ansys Mechanical available inputs

[ValentynBarannik]

Good day,

I'm truing to find the way how to get inputs (boundary conditions) from Ansys Mechanical to replace the values of them on the new one and perform calculation. the approaches I saw before were based of manual finding the values in ds.dat file. Is there any way to automate this process, like loading project file and recognition will provide me all data (boundary conditions) can be changed for simulation? If yes, could you recommend what file type should be used (*.dat, *.cdb, etc)

Thank you in advance.

[germa89]

Hello!

For changing things such as boundary conditions given a ds.dat file, you have two approaches if you want to use PyMAPDL:

• Run the ds.dat file using mapdl.input. Then you will have all the model in memory. Then you can change things, like boundary conditions using MAPDL commands such as mapdl.d, mapdl.f, etc. You should have also the components, so it should be easy to reuse them to apply/modify loads.
• Replace in the ds.dat file the hardcoded values. You can open ds.dat file within python (open("ds.dat", "r") as ...), replace/modify the lines you want, and then submit the job to MAPDL using mapdl.input_strings.

I'm afraid there is not a more dynamic approach with setters, getters, and classes in PyMAPDL.

Alternatively, you can have a look at PyMechanical using "embedded instances`.

[ValentynBarannik]

Hello German,

Thank you for the response.
Please correct me if I am wrong. So there is no way for now to "scan" Mechanical project/file and automatically determine the inputs and outputs of simulation that were specified by User in Mechanical UI by setting up the calculation. It is possible to do only in the case if User knows the location (node) of boundary condition. In this the case for User that is not experienced in Mechanical, there is no chance to set up automated workflow with boundary conditions varying and without deep diving into the structure of ds.dat(although I'm not sure that *.dat file is most suitable for this goal)

[germa89]

Hi @ValentynBarannik, I am afraid you are correct.

PyMechanical might help you on this.

[ValentynBarannik]

thank you,
so far I was not able to find the required functionality in PyMechanical

[germa89]

I would consider to open a discussion in their repo :)

[mikerife]

Hi @ValentynBarannik & @germa89
I thought maybe some additional information might help here. Even if it is way too late now. Anyway Mechanical APDL has some rules on parameter and component names. The first is that Ansys Inc reserves names that start with an underscore character to be an 'internal' name. Some APDL commands are actually APDL macros (files written in APDL). And to help avoid name conflicts they use leading underscores. Now WB Mechanical will do the same when applying loads and boundary conditions. Say a boundary is defined for a face in Mechanical. The MAPDL input file it is writing does not include CAD, so first a component is created of the nodes on the surface and given a name that starts with a underscore. Then the command to define the boundary condition will use that component name as the set of nodes to apply to instead of node numbers directly.

If you look at the input file written by Mechanical there is a comment given that describes the type of bc/load.

If we list the component in MAPDL or PyMAPDL then the those with the 'internal' name style will not be listed. But if instead of CMLIST we use CMLIST,ALL then all the components are listed. Maybe @germa89 can add the .to_list method to the PyMAPDL version of CMLIST with an option for 'ALL' we can see them.

Now if you are using Mechanical to pre-process the model then want to take it into PyMAPDL to set up the loads/bc's and solve. Or maybe solve multiple times for different loadings, you would be better off defining Named Selections in Mechanical of the regions you want to apply loads/bc's to. Give then a name that makes sense to you...like "Loc1FixedXYZ" or something. Then define and change the loads/bc's in PyMAPDL as needed with the component names. Then use the manual method in Mechanical to write out the input file.

Instead if you use PyMechanical you can turn on the recording of actions in the Mechanical scripting window, then define the load/bc. This will show the Mechanical commands used to define the load/bc. Then in PyMechanical you can reuse these and do a Python substitution on the values as needed.

Mike

[germa89]

The limitations on parameter names are documented here:
https://mapdl.docs.pyansys.com/version/stable/user_guide/parameters.html#specially-named-parameters

[germa89]

Creating #2560 to track possible improvements to CMLIST