Learning Forum

[yang]

Hello!

 

I would like to model cable-roof structures. Since only tension force will be found in the cable-roof structure, I use Link180 to model the cable. My question is how to show the axial stress of Link180 in Workbench, Mechanical application?

 

Thanks! 

[peteroznewman]

You could request Beam Results > Axial Force, and divide by the Area to get the Stress.

You can do that in a User Defined Result where I show dividing by an area of 0.001 m^2 in this example.

[jj77]

Happy Easter to everyone.

 

It is very easy, go to tools (see marking below), and insert beam tool, and look on direct stress which is the axial stress (Faxial/Area).

 

 

 

 

[yang]

Hello!

 

Thanks for the suggestion. I've tried, but because the element type is changed from beam to Link180. This is not workable for Link180. 

[yang]

Hello!

 

Thanks for the suggestion. I've tried, but because the element type is changed from beam to Link180. This is not workable for Link180. There's an error says "The result data for BEAM is not contained in the result file."

[peteroznewman]

Hello Yang,

Beam Tool > Direct Stress did not work for me either.

But the User Defined Result did work for me.  
You might need to set the Output Controls the same as I used.  It may be the General Misc. output.

Note: the real area of the cable in this model is 1.2566e-05 m² while I used 0.001 m² for an example.

ANSYS 19.2 archive attached.

[yang]

Hello, I will try. Thanks. My version is 19.1. Cannot open the archived file.

[jj77]

Must have been using a beam. It is very strange that it is not easier to get axial stresses out in a truss - if I ever work for Ansys I will look into this

 

Anyhow, the most reliable way to do this, as Peter said, is by using user defined equation, but use: = SMISC1/SMISC2 (Axial Force/Area), because in the other way one needs to get the area correct (if typed manually) - here though with SMISC2 it will pick the correct area for that element.

 

See help and link180 for more info on SMISC1 and 2

[vaibhavtaranekar]

Hi, Thanks for the command. Is there any way to get axial strain for link180 element?