Nonlinear Buckling in Ansys Help

[DerekGibson]

Hi everybody,

I am using Ansys V12.1 to do a nonlinear (GMNIA) analysis of a thin aluminium cylinder under axial load as per EC9-1-5. I have set up the geometry as a surface body and setup the static structural and linear buckling branches and everything works fine. Once solved I have transferred the results to mechanical APDL and written the following command line and used it as an input file:

/prep7
upgeom, 1 ,1,1,file,rst
cdwrite,db,file,cdb

Updating the MechAPDL branch works without any problems so I have transferred the MechAPDL to a new FEModeller. Within the FEModeller though the surface body geometry has shrunk by a factor of 1000? So instead of having a 3m diameter cylinder I have a 3mm diameter cylinder.

I cant for the life of me find out whats going wrong, is there a command in Mechanical APDL that can factor the geometry of the input file? I cant find any reference to this sort of problem in the Ansys literature or on the web. Has anybody encountered this problem before?

Do I need to use this method to use the deformed geometry from the linear buckling analysis as the imperfection value for out of roundness geometry in the GMNIA analysis.

Any help would be immensely appreciated.

If you need anymore information please ask.

Thanks

Derek

 

[Drej]

It may seem an obvious remark, but it sounds like a units problem (metres to mm).

Check the output of the cdwrite command - what are the model units? Does FEModeller have the option of flipping between unit systems?


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Drej]

Another thought: try also importing the model back into ANSYS classic and check the model units in there.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[DerekGibson]

Thanks Drej,

I have found a way around it by putting the prep7 command straight into solution branch of the linear buckling analysis then transferring directly into the FEmodeller. As far as I can tell its exactly the same process but this works and the other doesn't.

I had tried changing the units in the FEmodeller but these were already scaled down so it is definately the MechAPDL thats affecting the model.

Now I just need to get the solver to converge when using large deflections, it gives me an error message saying that this type of analysis is conflicting with the boundary conditions, I'm using a fixed support at the base and a displacement support allowing compression at the top of the cylinder, do you have any ideas what could cause this conflict?

Thanks for your help

Derek

 

[DerekGibson]

False alarm on fixing the geometry I'm afraid,

The MechAPDL is still scaling down the model. Where do I find the options for the CDWRITE command in APDL?

My units in workbench are in meters, if I transfer the setup from the Linear Buckling analysis to a new FEmodeller the geometry remains correct, its only when I transfer anything into MechAPDL that the geometry is affected. Even if the units in MechAPDL are set to mm I wouldn't expect it to scale down the model, is there a scaling feature in MechAPDL that could be doing this?

Any help with this would be great as I'm back to square 1

Thanks

Derek

 

[Drej]

Derek,

I'm a little confused about the route you're taking here.

Are you:

1.) Building and solving in Workbench
2.) Issuing an APDL branch in Workbench and writing out the updated geometry using upgeom and cdwrite as above
3.) Then bringing this deformed model into FEModeller

What's also confusing is your terminology. You mention "geometry" throughout - do you actually mean geometry (surfaces, lines, etc) or FE Model (nodes, elements)?

You should try and bring the updated model into ANSYS Mechanical (not Workbench) and check the units in there - ie by issuing a cdread of the cdb file you created. Also try setting the units before you cdwrite the model out - you can do this in Workbench.

The cdwrite command isn't clever enough to scale the model, however the upgeom does allow scaling, but I notice you are scaling using a factor of 1. You're also using the first set of results to update the geometry, yet this is a non-linear analysis and presumably has many sets on the results file.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[DerekGibson]

Drej,

The route you outlined is correct, but from the FEModeller I am transferring the deformed geometry into another static structural where I can re-apply the boundary conditions and loads etc and switch on large deflections and allow non-linear material behaviour.

The process I am following is that shown here:

http://www.edr.no/blogg/ansys_bloggen/ansys_tutorial_non_linear_buckling

By geometry I mean the actual model body (Surface Body), I have a 3m diameter cylinder throughout the workbench but a 3mm diameter cylinder following the MechAPDL process. I have set the units in workbench as you suggest but the same thing happens.

Your right, I am using the 1st buckling mode results from the initial analysis as the value for the out of roundness imperfection that is part of this type of analysis.

I have tried to read the .cdb file as you suggested but I cannot view units anywhere, I have tried adding keypoints and measuring between these but it just comes up as 3(doesn't tell me meters or millimetres).

As you might be able to tell I am a relatively new user of nonlinear aspects of Ansys and MechAPDL is totally new to me, is there anyway I can view the settings of the Upgeom function to see if this is scaling the model?

Thanks for your help

Derek

 

[Drej]

Ah.

Your model is correct by the sounds of things. You say you've measured the keypoints in ANSYS and it came back with a distance of "3", which is correct. 3 units long (or whatever).

There is no in-built units system here, only what the user defines. Don't forget that it is the responsibility of the user to set a consistent model unit system. Your model started as 3 units and is still 3 units. FEModeller is probably just set to "show" a units system of mm as opposed to meters that's all. It is up to the user to maintain his/her units system.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[DerekGibson]

Thanks for your help Drej, I'm gonna get on with it now and see what results I get, if it starts doing anymore weird and wonderful things I'll post it up here, its a very good site.

Thanks again

Derek