Ansys APDL Programming buckling FEA C Section Cold Formed Steel

  • Last Post 26 November 2018
  • Topic Is Solved
tanmaynade posted this 26 October 2018


I am facing issues with my program. Listed below. This is form my masters project. Also in what way can I connect the filleted surfaces shown in fig by a weld or just load or stress transfer connection. The link to the program is





Order By: Standard | Newest | Votes
Vitaliy_Degtyarev posted this 27 October 2018

You can find more detailed descriptions of the issues in the jobname.err file in the working directory. When I ran your code, I got a warning about only one element violating shape warning limits. The following description was given:

Quadrilateral element 41288 has a pair of opposite edges that are      
 77.42 degrees away from being parallel.  This exceeds the warning      
 limit of 70 degrees.

You can still run the analysis with this warning, but it is better to change the mesh. I usually select lines and divide them as needed using the LESIZE command, after which I mesh my models using mapped meshing (the MSHKEY command). With this method you have more control over the mesh and get a nice mesh with only rectangular and square elements. You may also want to have smaller divisions for the radii.

If your connections are discrete, you can couple displacements of the nodes that need to be connected using the CP command. If the connections are continuous, you could specify bonded contact between the surfaces.

Hope this helps.




  • Liked by
  • tanmaynade
tanmaynade posted this 23 November 2018

how to do bonded contact

rgpatchi posted this 23 November 2018

Hello Tanmaynade,

I have created a simple example to create contacts between two blocks in apdl. It is well commented. You can understand the basic procedure here and can further apply it to your model.    Also, please go through the help documentation for more reference on any commands used in the script. 


block,0,1,0,1,0,1 !make two blocks touching each other

et,1,186 !define a solid element type 

mp,ex,1,100 !define some elastic material properties

esize,0.2 !element size

vmesh,all !mesh all volumes

et,2,174 !create contact elements
keyopt,2,12,5         !bonded contact

r,2 !real number for this contact pair

et,3,170 !create target elements

asel,s,,,6 !select contact area
nsla,s,1 !select nodes attached to this area
esln !select elements attached to the selected nodes
type,2 !set contact type number
real,2 !set real number for contact pair - one real number for each contact pair
esurf !create contact elements on selected nodes

asel,s,,,11 !select target area
type,3 !set target element type number
real,2 !set real number for this contact pair
esurf !create target elements



nsel,s,loc,x,0 !constrain one end of block 1

nsel,s,loc,x,2 !apply displacement on other end of block 2


plnsol,u,x !plot disp x

You can also do this process via ANSYS Classic GUI using Contact wizard. 

Hope this helps. 

Best regards,


  • Liked by
  • SandeepMedikonda
  • tanmaynade
tanmaynade posted this 23 November 2018

thanks a lot

tanmaynade posted this 23 November 2018

also, I'm not able to create e proper mesh for my original program some elements get out of shape?


rgpatchi posted this 26 November 2018

Hello Tanmaynade,

Please provide some mesh sizing controls (to refine the mesh at these areas) to get a proper mesh. Also, posting an image of your mesh, where the elements get out of shape would help us provide better suggestions.

Best regards,



  • Liked by
  • tanmaynade
SandeepMedikonda posted this 26 November 2018


 Please create a new discussion for your question. This discussion is closed. Take a moment to review the guidelines on the Student Community.