December 20, 2018 at 4:35 pmneomale89Subscriber
I am trying to perform an analysis on a fuel tank which is been secured to the structure with the help of the straps. For the initial setup, I have not provided any material properties and also no hydrostatic load. I have also suppressed a few members to reduce the solving time. Attaching the archived model prepared in 18.2. Please help.
December 20, 2018 at 6:26 pmSandeep MedikondaAnsys Employee
Can you provide snapshots of your setup (boundary conditions), materials, model etc?
I am probably missing something but how can it solve without any materials or loads?
December 20, 2018 at 6:54 pm
December 20, 2018 at 7:22 pm
December 20, 2018 at 7:27 pmpeteroznewmanSubscriber
I set the number of steps to 1, since you only have one load, gravity. However, the solver will not converge in 26 iterations with 100 substeps. If you look at the NR Force Residual, all the points are around the brown strap.
Here is a closeup on the geometry
Here is the mesh
Here is a better mesh made by putting a Sizing Mesh Control on the 8 edges at the bottom of the strap.
While you are in the area, you can also add a Sizing control to the face of the solid part that the strap holds onto. That was too coarsely meshed also.
While a better mesh (on all four straps and Tee bolts) will allow the convergence to continue, it would be ideal to midsurface the straps. Do you want to do that while you are fixing the next issue?
The next issue that prevents convergence is the interference between the large light grey sidewall and the darker grey strap backer. The solver is trying to resolve that interference. Do you want to resolve it in the geometry editor and get rid of that interference? Then the model should converge.
December 20, 2018 at 7:29 pmneomale89Subscriber
Thanks, Peter. I will try to resolve the model again by implementing the suggestions above. Just one question, what are the substeps required in this case? How do we decide the number of substeps?
December 20, 2018 at 7:30 pmSandeep MedikondaAnsys Employee
What are the errors?
If the materials are not a problem. It is very likely coming from the contacts.
Also, what are your analysis settings?
I see that you did a modal analysis. Remove the Fixed support and perform an unconstrained modal analysis, what do you observe for the first 6 modes? Is something flying away? Try the methods listed here to debug.
Guidelines on the Student Community
December 20, 2018 at 7:34 pm
December 20, 2018 at 8:29 pmpeteroznewmanSubscriber
Neomale, you did a great job and hit all the right points trying to get this model running.
- NR Residuals
- Modal check for contacts
- Contact Tool
- Simplifying loads to get something to converge
You just need to learn to respond to NR Residuals with a mesh refinement and you will be a bit more capable
December 20, 2018 at 8:44 pmpeteroznewmanSubscriber
One idea to save you some time in the Geometry editor fixing the interference. Just remove that one strap face (actually 4 faces) from the contact definition so that the solver is not checking the faces that penetrate the tank. All the other faces of the strap that wrap around the tank are fine.
December 21, 2018 at 2:41 ampeteroznewmanSubscriber
I implemented the idea from my last post.
Now the NR Force Residual shows a problem on the No Separation contact.
Here is the No Separation contact.
I don't understand why a No Separation contact is used here.
Why not use a Bonded Contact so that the Tee bolt stays at its current location on that midsurface plate?
December 21, 2018 at 2:51 amneomale89Subscriber
yes I faced the same problem, the idea behind that was once the initial model is finalized, I want to put the initial tension in the belt to hold the tank steady. So I used no-separation to allow the movement along the axis of T bolt. I am not sure if this is the right approach.
So what I did was, I converted the following contact as bonded. I am still running the model, so can't comment on the results.
December 21, 2018 at 3:08 am
December 21, 2018 at 3:12 amneomale89Subscriber
Ohh, I didn't really see that. So what will be the best method to fix that? Should I go back in CAD model and fix that or is there any way of doing it in ANSYS workbench?
December 21, 2018 at 3:30 ampeteroznewmanSubscriber
All your geometry is in SpaceClaim, so you could try to use the Move tool to move those faces of that part up, while leaving the faces around the Tee bolt in place. This is complicated because there is the strap and the pad under the strap that both have to move. What if you just delete the pad from the model, and just have a strap?
You might have more control in the native CAD but then you will break a lot more of the model in Mechanical.
December 21, 2018 at 2:33 pmneomale89Subscriber
Good morning Peter,
So what I did is that I didn't make changes in the interference geometry and changed the contact formulation to the pure penalty, It converged.
Now I have introduced the material properties as shown below:
So, I want to know if it will be ok to use the pure penalty formulation with neoprene?
Also, if I want to introduce the tension in the belt, what will be the right way to do that? Right now what I am doing is applying force at the bottom of T- bolt, I don't know if it is right or wrong?
December 21, 2018 at 2:35 pmneomale89Subscriber
Ohh, so the image up there is blurry, adding more information the belt inside is steel, outside strap is neoprene and tank is steel.
December 21, 2018 at 4:46 pmpeteroznewmanSubscriber
Pure Penalty is a good contact formulation, it takes a little longer than the Default formulation, but if the Default fails, that is an excellent reason to try Pure Penalty. It's good for steel or neoprene.
Applying force to the T-bolt is good as long as it has freedom to move. If you changed the No Separation contacts between the T-bolt and the plate with the hole in it to Bonded Contact, then the T-bolt can no longer slide and the Force is not tensioning the strap. Instead of No Separation Contact, suppress that and insert a Translation Joint between the T-bolt and the plate with the hole. Make sure the X axis points along the length of the T-bolt. You then apply a Joint Load of Force to the Joint.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- How to calculate the residual stress on a coating by Vickers indentation?
- Solver Pivot Warning in Beam Element Model
- An Unknown error occurred during solution. Check the Solver Output…..
- Errors – Reinforced Concrete Beam
- 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
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Saving & sharing of Working project files in .wbpz format
- Colors and Mesh Display