Tagged: contact, forcereaction, meshgeneration, staticstructural


May 7, 2021 at 9:55 pm

May 10, 2021 at 7:37 am1shanAnsys Employee1) Is it possible to make the sphere a rigid body? No its not. You could try doing setting the behavior to rigid, you will observe that you cant scope the body to any kind of support.
2) Although the sliced model represents a 360 degree symmetry, the forces are calculated only for the edge that is scoped in the reaction probe. And since the edge you have specified is inclined, the force is also inclined. If you scope the reaction to the vertical edge, you will find that the horizontal components of both cancel each other, meaning the net force is in thee vertical direction.
3) For achieving a smooth transition you could try inserting an edge sizing with a bias factor or inflation layers with smooth transitioning. However, I think the sphere of influence should work just fine to give accurate results.
4) Well, if you have a singularity (point load corner etc.), this would mean that the stress would go on increasing as you decrease the mesh size, not matter how fine of a mesh you use, it will not converge. In such a case you will need to make certain modifications to your geometry (add filets) or loading (distribute the load over an area). Have a look at this article which explains singularity in detail https://enterfea.com/stresssingularityanhonestdiscussion/.
Regards Ishan.

May 10, 2021 at 8:41 amLorenzo98Subscriber, thank you for your answer.
1) Got it.
2) I'm sorry but I think I didn't understand. I scoped a perfect horizontal surface, not an inclined one. I tried to probe the reaction force on bot vertical edges like you say, but the horizontal component of the force didn't cancels out. Maybe what are you saying is that I'm interested only in vertical component of the force since, for symmetry, the horizontal component cancels? All I want from my model is the true vertical reaction force of the symmetric 3D case.
Applying the mathematical model to my project I find that the significative force is the vertical component, since with this component the theoretical calculations seem to agree, namely, the horizontal component cancels when I integrate over 360 degrees. Do you agree? Is this what were you saying?
3) Sphere of influence + growth rate seems good.
4) Thank you for the link.
I attach my project so maybe my doubts are more clear.

May 10, 2021 at 10:41 am1shanAnsys EmployeeHow have you applied the force in your simulation? The 2 images that you provided look to be different in terms of application of the force. In the left one the force is along the central axis, while in the second one it is on a offset distance. Both these cases are different. "... namely, the horizontal component cancels when I integrate over 360 degrees. Do you agree? Is this what were you saying?"  yes this is what I meant.
Regards Ishan.

May 10, 2021 at 10:32 pmLorenzo98SubscriberI haven't applied a force to be honest, but a vertical displacement (scoped to the upper flat edge of the semisphere) to which correspond a certain surface force (i.e. pressure). You're right, the pic I provided is a little bit misleading. Anyway, ok, the important thing is that I have to consider just the vertical component of the total reaction force vector.
Could I kindly ask you another thing? I'm having serious troubles to find the results that the theoretical mathematical model predicts (the Hertz contact model). I've already put myself in the physical condition to be sure that the theoretical model is valid. When I indent the sphere into the plane and plot [vertical component of the surface reaction force VS indentation] I should obtain a power law like F= k(E)*indentation^(1.5) where k(E) is a prefactor containing the Young's Modulus. What I've obtained so far is an exponent oscillating between 1.45 and 1.47 (depending on the mesh and other nonlinear parameters). The first thing I've thought was a problem of the mesh or nonlinear analysis, but after have tried everything the exponent still oscillates between 1.45 and 1.47, so I'm lost.
The theoretical model is: F = 4/3*E/(1v^2)*sqrt(R)*x^(1.5).
where F = normal force applied to the sphere which indents the plane, R = radius of the sphere, v = Poisson ratio, x = indentation (that is, the surface plane deformation along the axis).
I've put Large Deflections on On, the solver preference on Mechanical Nonlinear, the contact is frictionless and the contact status is closed. I also used Nonlinear Adaptive Region to take into account any bad mesh deformation. The material of the sphere is Structural Steel; for the plane I've created a simple elastic material with density 0.97 kg/m^3, E=0.5 MPa, v=0.49 .
The vertical component of the force data are reasonable, It means that applying the aforementioned equation to compute F for a given indentation X returns values very similar to those of the simulation. But, there is a but, the fit still gives me a coefficient of x different from the theoretical 1.5 :
Have you any idea? Thank you.
Best Regards

May 11, 2021 at 4:43 am1shanAnsys EmployeeCould you plot a least square error fit for x^1.5 and see how much the difference is? Also from the first image it looks like the deformation is large and thus not consistent with the small strain assumption. You may want to reduce your displacement to a very small value and then check the trend. Also, If you are comparing your simulation with a analytical solution based on linear elastic assumption, it would be better to switch large deflection off. I hope you are using a very fine mesh near the contact. The sphere of influence would be best suited for this problem.
Regards.

May 12, 2021 at 8:33 amLorenzo98SubscriberI've tried everything, It seems I can't obtain a perfect exponent of 1.5. If you think about it, it's reasonable since I'm simulating a real system with intrinsic computational limitations (finite mesh size, solving algorythms, etc) and I can't expect to obtain a perfect agreement with theoretical models. For my purposes, at the end, I obtain a reasonable value for the Young's Modulus within error of 2%.
One question: is it possible to use the Adaptive Convergence tool with probes? I want to track the mashbased convergence of my reaction force, but It seems I can't add this tool under Force Reaction in Solution section.

May 12, 2021 at 12:17 pm1shanAnsys EmployeeI don't think you could define convergence with any kind of vector result. However, you could automate the process by parameterizing the element size (input) and the force values (output).
Regards Ishan.

 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 lifesaving 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.
Ansys Blog
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

2092

1744

977

762

423
© 2022 Copyright ANSYS, Inc. All rights reserved.