April 26, 2018 at 5:27 ammauryaSubscriber
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.
April 27, 2018 at 11:42 ammauryaSubscriber
hello Peter sir
I solved the problem with link180 element but i have doubt in result, please check it.
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
April 27, 2018 at 12:06 pmpeteroznewmanSubscriber
Downloading now and will check it out.
April 27, 2018 at 2:14 pmsk_cheahSubscriber
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.
April 27, 2018 at 3:04 pmmauryaSubscriber
thankyou Now going to review the model sent by you.
April 27, 2018 at 3:36 pmmauryaSubscriber
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
April 27, 2018 at 5:23 pmsk_cheahSubscriber
- 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.
April 29, 2018 at 4:01 pmpeteroznewmanSubscriber
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!
April 29, 2018 at 4:26 pmmauryaSubscriber
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.
April 29, 2018 at 4:56 pmpeteroznewmanSubscriber
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.
May 1, 2018 at 4:40 ammauryaSubscriber
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.
May 1, 2018 at 9:28 ampeteroznewmanSubscriber
When I tried to run the Modal analysis with the ligaments, there were no results. I'm glad you got a reasonable result.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.