[AS_Aero]

Hi All

I am doing a simulation with particular physics, expressions, output control etc etc. I also export the ccl. Now when I change the geometry and do the meshing and if I want to have the same physics as my previous one, how can I achieve it ? Now I am setting up all the physics and experssions again one by one. But would be great if someone can help me to solve this somehow.


Also is there anyway in Workbench that I can run design parameter based simulation where I want to run in the cluster or server remotely

[Gert-Jan]

If you can export the ccl, you can als0 import it, not?

Alternatively, go to Pre. In the tree, look for "Flow Analysis 1", use your RMB and select "Edit in Command Editor". Now you see all your settings in text.
Delete everything, go to you text/ccl-file, copy everything and paste it in the Command Editor, and press "Process". Et Voila.

[-Maxim-]

as Gert-Jan said, you can either save/load the *.ccl files or if you would like some more manual work, you can copy&paste your expressions, monitors, etc via right-click on expressions etc. "edit in command editor" then mark all and copy that to your new project.
It helps of course if you keep the naming scheme the same as before so that your monitors point to the right expressions and right patches.

How did you survive that long without that?

[AS_Aero]

Hi Maxim

Till date I wasnt in need of repeating the same setup with lot of monitor points and expressions. Now I have some geometry variations but rest everything is same..so I dont want to create the expressions and monitor points and all the setups. So wondering about the ways to use this ccl file. I can import/export the ccl file so I will try that way.

[-Maxim-]

I see. I often have to do geometry variations so handling ccl-files is the "normal every day routine" for me. If you need help with that, just let us know.

[Opaque]

If you are working on a template problem, say a rotor, and you are changing blade profile.

You do not even need to export/import the CCL, just "Reload Mesh" feature. The new mesh is imported, and the CCL is properly attached to it.

Here is how it works:

ANSYS CFX separates mesh topology from physics topology, reason why you are in need to select mesh names, Location parameter, when creating a domain/boundary/sub-domain/etc and associate a new name, physics name.

That means, you can reload a mesh that uses the same "mesh names", and the physics is still valid. For example, if you have a rotor passage with mesh names: blade, hub, shroud, inlet, outlet, per1, per2, and reload a box with a standing plate using the same names as before, the physics will still be the same and you do not need to repeat any steps.

If you are working outside Workbench, set yourself up for this approach by using "standard for you" naming convention and stick to it.

Setup your case with all the bell and whistles

Write a definition file, compute results

For design iterations, Modify your geometry, remesh it, reload mesh, write definition file, compute results.

If you are in need to create new "surfaces" at the geometry level, the mesh will contain newer/different names, then the reload mesh will partially work and you need to correct manually.

Good luck