Simple Tension only Truss

  • 32 Views
  • Last Post 2 weeks ago
  • Topic Is Solved
learn13 posted this 2 weeks ago

Tension only link180 elements from beams within workbench v.19 are proving troublesome.

I've attached a version I've attempted and was hoping for some pointers on what may be going wrong.

 

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

One of several things that is wrong is you have many links along each line body. That doesn't work, especially for links in compression.

To correct that, click on the Mesh branch in the Outline. In the Details window, for Element Size, where it says Default, type 400 inches and remesh. Now you will only have one link on each line body.

In 19.2, you can change Beams to Links inside Mechanical without using APDL code, which is where you made the change.
Change the Model Type to Link. (If you shift-click, you can do four at once).

Not sure why you have Bonded Contact between the two cross-members. I expect that was automatically created by Workbench and you didn't notice it was there. You can suppress that if you don't want it.

Another problem is you don't have sufficient constraints to have a Static solution. You have only one Fixed Support. You need another vertex to have a constraint in the X-Y plane. 

I changed Displacement 2 to provide the four vertex corners a Z=0 constraint, while leaving all others free.
To allow it so solve, I added an X=0 Displacement Support at the top left vertex.

Did you confirm that your Mesh Edit merged 4 nodes?

With all the above changes, and if I suppress your Command Object, the model solves.

But if I unsuppress the Command Object, the code in it causes the Solver to fail.  Here is that code for other Community members to look at:

  • /gopr
  • allsel
  • *GET,maxsec,SECP,NUM,max,
  • *GET,maxetype,ETYP,0,NUM,max,
  • allsel
  • /prep7
  • esel,s,mat,,rope
  • *GET,xsec,SECP,matid,PROP,AREA,
  • ET,maxetype+1,180,,,1,
  • SECTYPE,maxsec+1,link,
  • SECDATA,xsec,
  • allsel
  • allsel
  • esel,s,mat,,rope
  • emodif,all,type,maxetype+1
  • emodif,all,SECNUM,maxsec+1
  • allsel
  • /nopr
  • /solu

Here is the error message in the Solution Output

 *** ERROR ***                           CP =       0.609   TIME= 12:52:09
 The section number must be greater than zero.                          
  Line= *GET,xsec,SECP,matid,PROP,AREA,                                 
  The *GET command is ignored.                                           

You can fix that and see if there are other errors in your code.

Regards,
Peter

learn13 posted this 2 weeks ago

@peteroznewman

Thank you for your reply and your help. I have access to v.19.0 and am unable to change from beams to links without ADPL.

With respect to the tension only aspect of the model, I found that it requires the large deformation definition to be turned on. 

 

Additionally, the links below can be used by those in the future to get started should they run into similar difficulties.

https://studentcommunity.ansys.com/thread/how-to-create-link180-element-in-tension-in-ansys-workbench/

http://www.ansystips.com/2018/04/tension-only-link180.html

https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_elem/Hlp_E_LINK180.html

Attached Files

Close