How to export a stressed body from one analysis into another in Ansys?
How to export a stressed body from one analysis into another in Ansys?
(OP)
Hello everybody!
Now are two months since I've been working with Ansys, more exactly Workbench 15. I need to know if there is possible to export a body from one static structural analysis into another static structural analysis so that I can constrain that body in other way(I don't need to change the mesh or anything else) and to keep the stressed state of the body from the previous analysis. Any idea would be greatly appreciated!
Thank you!
Kind regards,
Marius
Now are two months since I've been working with Ansys, more exactly Workbench 15. I need to know if there is possible to export a body from one static structural analysis into another static structural analysis so that I can constrain that body in other way(I don't need to change the mesh or anything else) and to keep the stressed state of the body from the previous analysis. Any idea would be greatly appreciated!
Thank you!
Kind regards,
Marius





RE: How to export a stressed body from one analysis into another in Ansys?
Rick Fischer
Principal Engineer
Argonne National Laboratory
RE: How to export a stressed body from one analysis into another in Ansys?
First of all, thank you for your answer. Perhaps I didn't made myself understood. I don't want to duplicate that same analysis, I want the stressed body(which has a plastic deformation) from the first analysis in another one without the loads and constrains that gave me the results so that I can subject it to other loads and constrain it otherwise, constrains that would be in conflict if they are in the same analysis.
Hope I made myself clear this time.
Thank you!
RE: How to export a stressed body from one analysis into another in Ansys?
Rick Fischer
Principal Engineer
Argonne National Laboratory
RE: How to export a stressed body from one analysis into another in Ansys?
RE: How to export a stressed body from one analysis into another in Ansys?
RE: How to export a stressed body from one analysis into another in Ansys?
Thank you!
RE: How to export a stressed body from one analysis into another in Ansys?
RE: How to export a stressed body from one analysis into another in Ansys?
In theory, there is no reason that you cannot run this as a single analysis, with multiple components advancing and retracting in successive load steps, but it makes things more complex. I cant see how to switch a displacement between free and a specified value in different load steps in WB. It might be there, I've just never needed to do this. Check with your tech support resource for help. Otherwise, setting up the solution phase might be easier with in MAPDL. If you click on Solution, then Tools, Write Input File, you will write the command script that WB submits to MAPDL to run the job to a text file. First, remove all your loads and boundary conditions from your model. Create named selections for any surfaces that you want to apply loads and BC's to. Then, open the file, strip out all the stuff after /Solu, and start typing. It might look something like this:
/solu
autots,on
nsubst,,,,,
Time,1
D,cylinder,ux,0
D,bush,ux,-2
solve
Time,2
ddele,bush,ux
d,bush,ux,2
solve
Time,3
etc.
Cylinder and bush are named selections from WB. Save the file, then open MAPDL, and do File, read Input from in the gui and run your file. This will require some knowledge of APDL commands. Also you would probably want to brush up on multi-frame restarts, so you don't have start the job over from the beginning if one load step doesn't converge. I've done stuff in MAPDL that was pretty complex, like forming of electrical connectors in a jack and then insertion of the plug, installation and removal of a tape mount where the tack strength of the tape during removal was a function of the application force, etc. Basically, you are limited by your imagination.
Also there is new at R14.5 a new customization tool in WB called ACT. I've never used it, but maybe there is something in there that could help.
Having said this, this is a lot of complexity for someone if they are not familiar with APDL. The smart thing is probably to go quick and easy first (i.e. run this as two separate jobs) and see what you get. Then, add complexity if needed.
Rick Fischer
Principal Engineer
Argonne National Laboratory
RE: How to export a stressed body from one analysis into another in Ansys?
Actually I've tried solving the problem by using other components instead of supports but, until now, I haven't managed to converge to solution just at the last step (something like 80-83%, when I get the message that the elements get highly distorted). Thank you again dear Rick, you've open up some directions!
Best regards,
Marius