how to create link180 element in TENSION in ansys workbench?

  • 697 Views
  • Last Post 01 May 2018
  • Topic Is Solved
maurya posted this 26 April 2018

hello sir,

                 i want link180 element for my analyses as this can work in tension only.

i want to design the ligaments which works in tension only and no effect on compression. 

In mechanical apdl file i learned that :

et, matid,link180 ! element type 

secdata,tenskey,1! it is the command to control the link either work in tension(1) or in compreesion(2)

but i didnot succeeded.

Please help

regards 

Deepak

  • Liked by
  • marviroso
Order By: Standard | Newest | Votes
maurya posted this 27 April 2018

hello Peter sir 

                         I solved the problem with link180 element but i have doubt in result, please check it.

file attached 

it is recognising element link180  but showing value of deformation of link in compression,but how to get stresses on link in ansys.

 

thanks waiting for response

              

Attached Files

peteroznewman posted this 27 April 2018

Downloading now and will check it out.

sk_cheah posted this 27 April 2018

I changed a few things...

  • seccontrol,,1  (not seccontrol,tenskey,1)
  • Model is not well constrained. Joint added to allow only for rotation. 
  • To avoid small pivot problems, density and gravity was added so the relaxed links won't be flapping in the wind
  • Analysis settings: Large deflection: On & Nodal Forces: Yes

I attached the tweaked model. 

 

Kind regards,

Jason

Attached Files

  • Liked by
  • maurya
maurya posted this 27 April 2018

hello Jason,

                    thankyou  Now going to review the model sent by you.

regards

Deepak Maurya

maurya posted this 27 April 2018

 hello Jason sir,

                          i have some doubt:

1) you replaced moment by joint moment,Why?

joint moment is wrt ground in particular direction similar to moment also (acted in particular direction)

2) direction of gravity is along the side of body in Zdirection (i think by mistake universal direction chossen)

My main aim is to use this link as ligament of human body for my analyses, ANY suggestion

regards

Deepak 

sk_cheah posted this 27 April 2018

Hi Deepak,

  • With an applied moment, the body will 'fly' until the string catches it, then do a few acrobatic somersault. It's tough for Ansys to converge on the flight path. The joint constrains the body to have a 1DOF that is controlled by LINK180. 
  • Imagine the string is in outer space with no gravity. When it is not in tension, it is simply floating around. To avoid this ill defined problem, a small gravitational force is applied. This should not significantly affect the attached body while helping convergence. 

Kind regards,

Jason

  • Liked by
  • maurya
  • peteroznewman
peteroznewman posted this 29 April 2018

Hi Deepak,

Jason explained this very well. Remember to add a Density property to the materials assigned to the LINK180 so that the gravitational force will have something to pull on!

Kind regards,

Peter

  • Liked by
  • maurya
maurya posted this 29 April 2018

Hello Jason 

                   one query i have ?

     the model you messaged me  is working nice but problem is this when you define Material properties as command in WORKBENCH it is not considering it.

the last model has steel as default material so density was feed previously. I created ligament material properties and didnot provide density in add material but i add density during command it is not accepting it.

Regards 

Deepak

peteroznewman posted this 29 April 2018

Hello Deepak,

The reason I posted above is because I added a Modal analysis to your New Beginnings file and found that there was no density assigned to the ligaments. I went in and added that in Engineering Data and am running the Modal now to look for loose parts.

Regards,

Peter

  • Liked by
  • maurya
maurya posted this 01 May 2018

Hello Peter sir 

                      i also performed the modal analyses yesterday for five vertebrae without ligaments and message the file to you but its fail as size cross 15 GB of my gmail. I just want  to tell that if you see the modal analyses of first five modes it shows the five physiological motion of human body 1)compression

                                                                                                                                                                                    2) forward bending

                                                                                                                                                                                        3) backward bending

4) lateral bending and so on.

i performed for five vertebrae.

thankyou

                                          

peteroznewman posted this 01 May 2018

Hello Deepak,

When I tried to run the Modal analysis with the ligaments, there were no results.  I'm glad you got a reasonable result.

Regards,

Peter

  • Liked by
  • maurya
Close