May 20, 2018 at 1:44 ampeteroznewmanSubscriber
Deepak Maurya has been working on a simulation of spinal bones and the disks separating them. Bone is a couple of orders of magnitude stiffer than disk material, so one model represents the bones as rigid bodies while the disks are flexible bodies.
Some protrusions from the bones slide on each other, so he has used frictional contact between them. Some diseases of the spine fuse those bones together. To simulate that, the frictional contact is changed to bonded contact.
Deepak asks why there would be any deformation in the disk if the rigid bones are connected with bonded contact. Rather than work on his very large model, I have a very small model.
It has two rigid bodies with a flexible block between them. The block between them is bonded to each rigid end body. One rigid block is fixed and the other has a force applied. There is also a frictional contact between the rigid bodies.
If the frictional contact is changed to bonded contact, this is the result.
The flexible body has practically zero deformation. Is this what you are seeing?
If not and the deformation with bonded contact is similar in magnitude to the frictional contact case above, then that is likely due to some conflict in the model, an over-constraint that makes it impossible for the solver to satisfy all the constraints at the same time and so some constraints are ignored in order for the solver to continue. When this happens, there are always WARNINGS in the output file such as this:
*WARNING*: Some rigid target elements (e.g.810) in real constant set 5
overlap with other MPC/Lagrange based elements (e.g.1123) in real
constant set 10 which can cause overconstraint.
The problem with a complex model is that there are likely to be many warnings, but most of them do not represent a true conflict. For example you can have separate contacts on adjacent faces of a block that gets bonded into a corner. The nodes on the edge of the block belong to two contacts at the same time, so a warning may be issued, but there is not an actual overconstraint.
The ANSYS 19.0 archive for the model above is attached below.
May 20, 2018 at 5:33 ammauryaSubscriber
In this analyses, after considering rigid body there should not be relative motion even in micron in actual.
Thankyou for that warning concept this warning i observed sometimes.
May 20, 2018 at 11:34 ampeteroznewmanSubscriber
This very simple model includes four warnings, including this scary looking one:
And in this case, there is no actual conflict.
The formulation of Bonded Contact requires some very small movement to generate an opposing force. But the ratio between the motion of the flexible block for frictional:bonded contact is 20000:1 which is adequate for most analyses.
If you need a perfectly rigid connection, then use a fixed joint. Below is the image where I suppressed the Bonded Contact and created a Fixed Joint. This is what you want, but it is more work than simply changing a pull-down menu from Frictional to Bonded.
Now bond a second flexible block to the rigid "L" part and move the fixed face from the rigid "L" piece to the base of the new flexible block and plot the deformation.
You can't tell from this plot of deformation if the first flexible block is being squeezed because it has a rigid body motion through space enabled by the second flexible block. To find out if there is any squeezing, plot strain instead of deformation.
Now it is clear that the fixed joint between the rigid parts is not allowing any deformation into the first flexible block.
I hope this clarified some concepts that apply to your complex spine compression and bending models.
Attached is an ANSYS 19.0 archive.
May 20, 2018 at 12:18 pmmauryaSubscriber
Thank you sir very nice
October 23, 2018 at 7:26 amRaajSubscriber
I performed a modal analysis of the above-discussed problem. In the total deformation, there is relative motion between the flexible and rigid body (one on which force is applied) though I have assigned bonded contact between them. Could you please explain why it is so?
Thanks in advance,
October 23, 2018 at 12:03 pm
September 18, 2019 at 3:59 pmAutonewbieSubscriber
I have a question about defining the contact between both rigid bodies. The models below have been simplified. I wanted to make the bottom part as rigid body to reduce the simulation time but when it is changed to rigid body, bonded contact will not be applicable as the screw (the round screw head) is also modeled as rigid body. Do you have any advice? Thank you so much!
September 18, 2019 at 7:23 pmpeteroznewmanSubscriber
Replace Bonded Contact with a Fixed Joint. Pick the small surface first to locate the coordinate system that locates the joint.
September 19, 2019 at 2:08 amAutonewbieSubscriber
Thank you Peter! Does it matter which part is selected for reference or mobile for fixed joint?
- 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?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- 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.