December 1, 2022 at 9:11 pmsafianaSubscriber
I am modeling a 2D plane strain model of a cylindrical roller bearing in ANSYS APDL. I have a bearing housing which inside it there is an outer ring with 5 rollers in its bottom half. Also, there is a thin layer of soft material between the outer ring and the housing. I want to apply 180 N force on the middle roller, 100 N on the left and right rollers closer to the middle, and 20 N on each roller on the far end (right and left). The length of the roller and bearing in the normal direction is 11 mm which I used "le" in my commands. So, the force on each bearing named by Q1 to Q3 must be divided by 11. Also, to apply these forces as pressure (SFL) on the surface of the rollers, I must divide these forces by the diameter of the roller which is 10 mm. Then, I apply these pressure on the roller and solve the model. The contact between the lower half of the bearing and housing is bonded, and the bottom half is frictionless. The soft material is already glued on the outer ring with AGLUE command. The contact of the rollers and the outer ring is rough and on the two corners of each roller I have constrained the rotational motion of the rollers to prevent rigid body motion (radial direction is free).
Now what I expect from solving this model is that if I type "FSUM" for the whole model, I should get a value equal to the total force I applied to my model. I applied 180 + 2*100 + 2*20 = 420 and divided by the length of the model (11 mm) will be 38.1 N/mm but I get 33.17 (if you write allsel and then type FSUM in the post-processing).
My main objective now is to see how much of these forces is being applied to the soft material between the outer ring and the housing. That is why at the end of my code I wrote asel,s,,,5,8 and I typed FSUM for these small areas. But it gives zero force to me. If I select the housing only and do FSUM, again it gives me zero. The only way I can see the force is when everything is selected.
I don't think this is true and there must be a reaction force between the outer ring/soft material and the housing surface. Does anyone have any idea?
December 2, 2022 at 1:19 pmChandra SekaranAnsys Employee
Use PRRS to check if the reaction forces match the applied loads.
FSUM works based on currently selected elements and nodes. 'asel' by itself does not select the nodes and elements. Also remember that the model is in equilibrium if the solution converges successfully. So sum of forces at a node (if all the elements attached to the node are selected) should be zero. So you may want to select the nodes at the interface and the elements of the soft material that are conneced to these nodes and do FSUM.
December 2, 2022 at 5:25 pmsafianaSubscriber
Thank you for your reply, but that didn't solve my problem. It is true that ASEL command is not enough. I already had used Asel and following that nsla,s and esln,s to make sure only nodes and elements attached to an area are selected.
If I select the nodes at the bottom of the model where I have fixed support, whether I select the nodes at the bottom or just the elements at the bottom, the FSUM command gives me 30 N force. But It doesn't happen if I select the elements on the soft material, plus the nodes on the interface surface which is the housing. That is the region where the bonded contact is happening and I thick the reaction force between the soft material and the housing surface must be equal to the applied load on the rollers. But it give me zero force again. How is possible that loads are applied to the rollers and the reaction force in the contact region is zero by FSUM command? I also selected the contact elements at this region to see if the contact pressure is as I expect. It looks logical that pressure is higher at rollers positions. So how it is possible my forces are zero at the interface region or on the soft material? Any help is greatly appreciated.
December 2, 2022 at 7:44 pmBill BulatAnsys Employee
Please try these commands:esel,s,mat,,2 ! SELECT THIN LAYER OF SOFT MATERIALnslecsys,1*get,r_inner,node,,mnloc,x ! INNER RADIUS*get,r_outer,node,,mxloc,x ! OUTER RADIUSnsle ! NET FORCES SOFT MATERIAL EXERTS ON INNER RADIUS NODESnsel,r,loc,x,r_innerfsumnsle ! NET FORCES SOFT MATERIAL EXERTS ON OUTER RADIUS NODESnsel,r,loc,x,r_outerfsumYou should see this if you're post processing interactively (the net FY values are equal and opposite, which I would expect of a static strautural analysis):
December 2, 2022 at 8:02 pmsafianaSubscriber
Wonderful! Thank you so much!
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.