November 28, 2019 at 5:49 pmKetsuiSubscriber
I have been trying to complete a relatively simple project in which i need to find the maximum stresses present on a bracket that is being subjected to a specified load. Unfortunately, generally, with increasing mesh density, the stresses increase exponentially, and this continues onward. I suspect i have an issue with the way the problem is set up in the program. In order to speed up the entire process of convergence, i have utilized adaptive mesh refinement, but even after letting the program run all night, there is no convergence whatsoever even though the program do come to a result with each loop.
I am also having plenty of issues uploading an image here...
Long story short, the program is modeled as an L bracket attached to the underside of a desk. A moment and a force is applied at the bottom of the L bracket, whereas the top is held up to the underside by the 2 screws. I have a rough contact connection between the L bracket and the desk, a bonded contact between the screw flange and the bracket, and a bonded contact between the screw and the holes within the "desk". I am expecting there to be stresses near the screws and maybe a very small deformation where parts of the bracket is lifted off of the desk due to the force pulling downwards (or not). I have increasing stresses occurring at the edge of the holes where the screws are supporting the bracket.
Hopefully, somebody can help. I've been working on this for a couple days now, and i've just about ran out of ideas.
November 29, 2019 at 4:20 ampeteroznewmanSubscriber
Good Evening Ketsui,
When the stress keeps increasing as the elements get smaller, that is called a stress singularity. It means the true solution is infinite stress. The simple example is a solid L bracket that has a 90 degree interior corner edge. By adding a blend radius to that corner edge, the stress singularity can be eliminated and the stress converges on a finite value as the element size is reduced.
Sometimes a bonded contact can create a stress singularity when it brings two parts together and creates a "crack" between two parts, like the 90 degree corner edge but at 0 degrees. The singularity can be eliminated by replacing the bonded contact with frictional contact. You don't want to model the threads on the screw and the hole, so Contact Details includes a Geometric Modification called Bolt Thread that lets you replace Bonded contact between a cylindrical solid and cylindrical hole with Frictional contact and "simulated" bolt threads that hold the "screw" into the "threaded" hole. Read the ANSYS help about this feature as there are meshing requirements like 4 elements per thread pitch.
The website is a little broken today, so no one is able to insert images.
November 29, 2019 at 4:59 amKetsuiSubscriber
thank you so much for replying!
after an *excessive* amount of research, i managed to figure out it was a stress singularity issue, and i managed dwindle my issues down to one problem: the bolt head on the bracket. It appears i am getting singularity on the bracket where the corner of the bolt head makes contact with it (even though i put a fillet on it as well). I have tried bonded, rough, and friction type contact, but in each case, i get increasingly high stresses that diverge with increasing mesh sizes. I have tried to decrease contact stiffness down to i believe 0.05, but im still running into this issue.
November 29, 2019 at 7:23 pmpeteroznewmanSubscriber
Create a Workbench Archive .wbpz file and attach it to your reply and say what version of ANSYS you are using, I will take a look at it.
November 29, 2019 at 7:30 pmKetsuiSubscriber
Okay, thank you very much!
Edit: I'm Using ANSYS 16.0
November 29, 2019 at 11:55 pmpeteroznewmanSubscriber
1) Add a blend (could be smaller than this) to eliminate a singularity on this edge.
2) Use the back of the block (one face) as the Fixed Support and no others.
3) This is optional, but is useful to speed up the solution, or to fit in the Student license limits.
Add a Plane at the center of the part and apply Symmetry in DesignModeler.
If you do this, you also have to divide the load in half in Mechanical.
4) Use Frictional Contact between the underside of the screw head and the bracket.
5) Use Frictional Contact between the Block and the Bracket.
6) Use Bonded Contact between the screw and bolt hole.
This could be Frictional with the Bolt Thread modification, but that may not be required to avoid a singularity.
Another idea is to split the shank face of the screw at the front of the block. Then Bolt Pretension could be used.
I don't use the Convergence feature much myself because I can't use Multizone meshing.
I have to solve this on my other computer because I hit the Student license limit on this one.
Here are the first six results, it seems to be converging.
November 30, 2019 at 5:34 pmKetsuiSubscriber
Thank you for your help.
So, i've one part of you solution and used only the back of the plate as the support and removed all the others. I'm trying to save on computational time so i didnt want to use frictional contacts and opted for bonded contacts. Also,the forces incurred on the bracket will eventually include a momentum force, so i can't use symmetry. That being said...my solution appears to be converging (finally). However, i have drastically lower equivalent stresses compared to you. Right now, im at 6.32MPa on the screw after 5 solutions (and ~0% change over the last 2).
Do you remember where your maximum stresses were occuring? If not, assuming that further convergence doesnt reveal additional singularities, i think i should be okay. Im certain i will have to add a fillet as i design the bracket to be thinner over time.
Thank you again!
November 30, 2019 at 7:05 pmpeteroznewmanSubscriber
Are you saying you have the bracket bonded to the block? That doesn't make sense.
The maximum stress in my mesh is occurring at the fillet of the screw head. That makes sense.
November 30, 2019 at 8:48 pmKetsuiSubscriber
nope. bracket is rough contact with block.
and the maximum stress for me was occurring at the same area...would the type of bonding make that big of a difference? would a bonding contact ignore shear stress along a plane?
edit: went out and got more RAM for my laptop, going to run another analysis with more elements...there's a chance my values were off. will update when i can
December 1, 2019 at 1:21 pmpeteroznewmanSubscriber
I reran the convergence with a slightly different mesh and I added a Stress result that was just on the screw body.
I got the following graph.
This is another reason I don't like the automatic Convergence tool. I don't have the control I want compared with doing a Mesh Refinement Study manually.
December 1, 2019 at 8:33 pmKetsuiSubscriber
I am very confused as to why our values for stress are so different. My maximum stress on the bolt is still around 100MPa. Is the force you're using still around 240N?
I managed to attain a converged solution on the first iteration of the bracket. Now on the second one with a smaller profile, I'm somehow getting singularities where the screw head contacts with bracket. This didnt happen with the first iteration after the changes you've recommended. I'm beginning to get very confused with respect to how contact is treated in ANSYS
edit: attempting solution with rough and frictional contacts on the flat side of the screws.
December 2, 2019 at 3:41 ampeteroznewmanSubscriber
Let me repeat, I don't like the automatic Convergence tool because it gives such wildly different results depending on the starting mesh and it stops after 6 iterations, regardless of whether the convergence criterion was met.
Also, as someone else asked, how do you obtain the last mesh used for another analysis?
I prefer manually controlling the element size and using the Parameter Set to automate the solving of models with varying element sizes. That way, you get to keep any mesh used, since you created it.
December 2, 2019 at 3:56 amKetsuiSubscriber
I completely understand. Automatic convergence tool tends to chase and give higher resolution/more elemets to whatever location that it found to have higher stresses. I have seen at times that with it, the location of maximum stress completely changed with each iteration, and then this throws whatever prior convergence out the window. It can be a pretty poor tool at times.
That being said, at the moment, i found use for it, as it definitely helped me isolate, find and understand the mechanisms behind singularities.
Also, following your first suggestion about turning the contacts between the bracket and the screws as friction force helped alot. Should've followed it from before. Thank you! However, what values would you estimate for the coefficient of friction?
December 2, 2019 at 4:02 ampeteroznewmanSubscriber
It's best when designing structures to build models that are conservative. That means models that give the highest (converged) stress. That typically means you should use the lowest conceivable friction coefficient. Frictionless sometimes has more convergence difficulties than frictional, but a coefficient of 0.1 or 0.05 for unlubricated surfaces is defensible.
Please click a post above with Is Solution to mark the discussion as Solved, or ask a followup question.
December 6, 2019 at 4:46 amKetsuiSubscriber
Sorry, got swept up with exam season.
Marked one of the posts as solution! and thanks again for your help, i greatly appreciate it.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.