Ansys WB10.0 -- cylindrical forced displacement 1

[hamster001]

Hello all,

Hope you can help me out with this one.
Using ansys workbench V10.0

I'm trying to apply a radial displacement constraint
on a cylindrical object.
I've managed to create a new local coordinate system
which resides at the axis of the cylindrical object.

In some way however, workbench does not accept any input
regarding the new coordinate system when inserting a displacement boundary condition.

I've also tried to attach the geometry item to the new
cylindrical coordinate system, however still no luck.

What am I doing wrong ?

 

[meshparts]

I don't know about Ansys Workbench but in Ansys classical you must roate the nodes into the cylindrical coordinate system and the apply the displacements in x direction (x is radial in a cilindrical system)

So I guess, you must find a way to rotate the nodes coordinate systems. This is very simple in Ansys classical: see nrotat comand.

Regards,
Alex

 

[hamster001]

Hi Alex,

Thanks for your update.

I was already considering moving my model into Ansys classical. I've had no luck yet with workbench.

The weird thing is, that it is actually pretty easy
to define a cylindrical coordinate system in workbench.
I've found out that the new coordinate system IS selectable
for force boundary conditions, displacement only seems to
take the global coordinate system.

I will checkout the nrotat command, but will have to dig in the past when working with classical again.
Fortunately, ansys workbench allow for exporting an ans file for ansys classical, so it should work pretty swift.

Regards.

 

[ansysfreak]

Hi

You can apply radial contraint by jusing the displacement Cylindrical Support. Here you can set, radial or axial or tangential, to fixed or free.

Hope it helps

Garry

 

[hamster001]

Hi Garry,

The cylindrical support constraint is used for constraining
cylindrical parts, however it does not allow you to
provide a value for the displacement.

Maybe I need to redefine my issue a little :

I want to expand a metal tube with some cutouts in radial direction. I expect that by doing this, the tube will get shorter and the cutouts deform.
Basically there are 2 issues here :

1. How to constrain this part ?

You actually do not have a fixed point somewhere, but the cylindrical support might do the trick. The problem is that radial and tangetial deformation must be allowed and actually also the axial deformation ! So this is pretty confusing.

2. How to apply external forces to achieve the correct results ?

The best approach to the actual proces would be to radially
expand all nodes with a certain value.
Applying a pressure on the inside wall does not give a good result as the actual deformation is also displacement limited.

One approach I'm looking at, is to use a much longer cylindrical object in the tube, expand this one and
use contact surfaces to enlarge the actual model.
This still requires radial movement constraints.

Any comments / experiences on this ?
Many thanks !

 

[ansysfreak]

Hi

Sorry I cant help you now I'm to dusy.

But you can solve this problem by jusing APDL in Workbench.
It's the same problem as in Ansys tratitional. Look at this thread:
Importing displacement boundary conditions.

grtz g

 

[cbrn]

Hi,
Ansysfreak is perfectly right.
Insert a "Command" object in the Environment for which you want to set your D boundary condition. In this APDL, you can insert the same commands that work in Ansys Classical, so in your case you'd have to write something like that:

/PREP7
CSYS,0 !sets a CSYS to start with (may not be global cartesian)
WPCSYS,-1 !sets working plane to the active CSYS
WPROTA,45,0,0 !this is an example only, of course: reorient the working plane as you need
CSWPLA,21,1 !creates the cylindrical CSYS #21 corresponding to the current working plane
CMSEL,s,MY_SELECTION_GROUP ! if you have predefined an adequate selection group, this will help you very much!
NROTAT,all !this will rotate all the nodes in the selection group to CSYS,21
D,all,X,RADIAL_DISPL_VALUE !apply the radial displacement

Don't issue a "/FINISH" command after your /PREP7 commands, otherwise the Workbench processing will be interrupted before it re-enters Solution (in fact, it does enter /SOLU before it will read your APDL placed in the "Environment" branch: this is for setting-up some internal parameters. But by issueing /PREP7 you force it to exit /SOLU and re-enter the preprocessor; after it has processed your commands, however, it continues with its standard procedure).

 

[hamster001]

Hi Guys,

Thanks a lot.
After Ansysfreak remarks I managed to insert the command object and used the cylindrical system (created in workbench) by manually giving it code 12 (so CSYS,12)
to rotate the nodes into it by using APDL.
Took a while before I figured out I needed prep7 to jump out of solutions mode, but this was actually reported in worksheet using a solutions information tool in the solutions objects (guess good reading is also an expertise ) .

Now it's up to the next step of correctly putting the other
constraints in place, but I'm progressing with it.

Thnks,
DB