How to export a stressed body from one analysis into another in Ansys? 1

[scarules2006]

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

 

[rickfischer51]

In the main project window, click on the analysis system you want to work on and hit Duplicate. Then open that system and make your changes.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[scarules2006]

Dear Rick,
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!

 

[rickfischer51]

Run this in multiple load steps. Load step #1, apply your first load case. Load step 2, remove your first load case. Load step 3, apply your second load case. Load step 4, remove the second load case. Remove the loads slowly to avoid convergence problems. Forces and pressures can be ramped to zero. Displacements should be ramped to near zero, and then set to free. Remember that a displacement set to zero is not the same as free. Depending on your model you may need two load steps to remove a displacement load.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[scarules2006]

Not the loads are my problem. Let's say that in the first step I apply a load and the body has on one face defined a fixed support. When I need to apply the other load scenario I must disable somehow the fixed support from the first step and I didn't found a way to define them as tabular data so that I could enable/disable them or any other way to do that (this is only as example, my analysis is more complex, I constrain the body by using another body and after that I need to remove the rigid body that was used to constrain and to deform the main body and on the face that was in contact with the rigid body I must define a support and other similar scenarios). Is there any way to enable/disable the supports in same analysis even by using more steps? Thank you!

 

[inline6]

drag another static structural (or modal etc) onto the MODEL at the main workbench page. this will allow different loads, Boundary conditions using the same geom, mesh, contacts, joints etc

 

[scarules2006]

Ok, thank you all for trying to help me. Let me explain exactly what I want to do. I have a bush, formed by 2 parts of metal and one made of rubber. The two cylinders of the bush are defined as Structural Steel NL, the rubber part is modeled with Neo-Hookean, curve fitted by uniaxial test data from my lab. The exterior cylinder of the bush has an external diameter of 90 mm. In this same analysis I have another body, a cylinder , made of Structural Steel NL but defined as rigid(the bush is defined flexible). The internal diameter of the rigid cylinder has a value of 89mm. In one step of my analysis I put the bush to go through the rigid cylinder and as result I get a stressed deformed bush, which now has an external diameter of 89mm instead of 90mm(operation that we call "calibration"). To do this operation I need to support the bush on the opposite side from which the rigid cylinder comes(I'm actually using also other constrains that would get in my way in the future of my analysis). For my next step this support gets in my way so I need to know if I can put in another analysis the bush already "calibrated" from this analysis but not to go again in the "calibration process", or to remove the constrains that are getting in my way if I continue the same analysis.
Thank you!

 

[scarules2006]

Any ideas? Thank you!

 

[rickfischer51]

This gets more complex with each post. If you conduct this as two separate analyses, you will not get in the second analysis the strain history in the bushing from the calibration step. Otherwise you can run this as two separate analyses. You need to decide if that is significant. The tangent modulus for that material is pretty flat, so hardening effects should be minimal.

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

 

[scarules2006]

Thank you Rick!
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