How to get longitudinal and circumferential stress and strain results?

[richonlinedeal]

Hello all,

I did some structural analysis in ANSYS, and Cartesian coordinate system was used.

I got all the stress and strain results in Cartesian system (the X, Y, Z components), could any people here advise how to translate them to Cylindrical components in ANSYS Postprocessing, i.e. get the corresponding longitudinal and circumferential results for stress/strain?

Thanks a lot.

Jerry

 

[Stringmaker]

This is easy. If your model has its axis about the global X, Y, or Z axes then you can just use a predefined coordinate system to post process with. CSYS 1,5,6 are cylindrical coordinate systems internal to Ansys. Issue CSLIST to get their specifics. The procedure you want to use is something like this:

CS !create a coordinate system if the predefined coordinate systems won't work (if your model does not have an axis about the origin)
RSYS !specifies which coordinate system results should be transformed with respect to
PLNSOL !normal /post1 commands can be used from here

I would advise reading the documenation about coordinate systems in general as well as the RSYS command. In a cylindrical coordinate system, X,Y,and Z correspond to R,Theta,and Z. So is you plot stress in the Z direction you are really plotting the axial components and so forth.

-Brian

 

[richonlinedeal]

Thanks Brian for your always helpful tips.

I actually did try CSYS to change the active coordinate system. But there were some problems:
1) My structure is tube with multiple asymmetric branches, and they don't have global X, Y or Z axis and origin as well;
2) Whether I used a predefined cylindrical CS or customer defined cylindrical CS, the geometry of the model got distorted when I plotted the results;
3) The range of magnitude for stress/strain result seemed to be the same in different CS, for example, Cylindrical and Cartesian. Only the model geometry get distorted.

I might miss some points, but can't figure it out. If you have any more comments, please let me know.

Thanks.

Jerry

 

[cbrn]

Hi,
make sure you don't mix up things:
- CSYS is for setting the active coordinate system (i.e. the coord sys used for interaction with the "model world")
- DSYS is for setting the display coordinate system. For display, never change it from 0 or you may straighten curved lines or other "strange" things on the viewport (you have to change it only in special cases, for example to list coordinates of nodes in a system other than global cartesian 0)
- RSYS is for setting the results coordinate system, i.e. the system in which the numerical results are evaluated. This one is what you seem to need.

Regards

 

[Lirock]

Hi,Jerry:
In fact, there is a coordinate system called 'result coordinate system',which is the globle cartesian cootdinate system by default.You can 'RSYS' command to change it to any other coordinate systems.
So,for your peoblem,you just need to build a cylinder coordinate system,and chang the result system to it. And then, X axe will be the radial direction,Y will be the circumferential direction, and Z will be the axial direction.
And what's more, if your model just fits the globle cylinder coordinate system,reference number 1, you can just use 'RSYS,1' and then you can check the longitudinal and circumferential results for stress/strain.
Hope this would help you!

Rock Li