Hey,
I'm currently modelling a helical gear pair in Static Structural (Ansys 19.1) to find the contact stresses on the teeth under a certain load. I'm also interested in the shear stresses just under the surface of the teeth, therefore I added the Inflation option to my mesh. However this option greatly increases the element count in my model. I attached a picture to show my current mesh. Depicted there is a section cut through both gears, to show the mesh on the inside.
I could of course just reduce the layer count of the inflation, but I'm curious if there is a better option to get a finer mesh on the inside. So the question would be if there is a better alternative to inflation to more finely mesh my parts just under the surface? Or is there another method to reduce the element count?
Regards
Paul
A good option, even not in Ansys., could be Transmission3D. It uses a rought mesh for taking into account the stiffness and deflection of the teeth while in the contact it uses a semi-analytical appropach based on the Hertzian theory.
Contact me for further details.
Franco
Dear Paul,
Inflation not only increases the number of elements but also increases the number of DOFs, resulting in a more lengthy simulation (Tetrahedral elements have fewer degrees of freedom than hexahedrons). In any case, extra care should be taken with inflation. Those elements have a very bad aspect ratio and they should be only used when the gradients in the in-plane coordinates are very small in comparison to the gradients in the cross-plane component. From the attached picture it doesn't look like you need inflation. Rather than using that approach probably I would use either a control volume or proper partitioning of the geometry to control the mesh size. For instance, you can create a control volume containing all the teeth and set a slower growth rate there (You start by sizing the elements in the teeth faces and from there a patch conforming method with 1.05 growth rate). In that way, you can have only 2-3 elements in the interior region where you have the inflation now, and that looks like it is enough to capture stresses in your problem.
Kind regards,
Julian
Hello Paul, you can use the volume sizing (by splitting the volume in pre-processor) for this case than using inflation, or a better sizing strategy will work.
I have seen people generally use inflation mainly in FSI kind of simulations to get the better results.
Thank you all for the answers! Volume sizing on just the teeth or just the faces sounds like a good idea, I will try that and report back.
I have to do this Ansys, so another program is unfortunately not an option.
Hi Paul Melzer ,
Can the geometry be spit to allow sweep meshing in the teeth and to have rough tetra mesh for the hub area?
Since sweep mesh uses mostly hexahedron it will significantly reduces element count.
Best Regards,
Rashiga
Hi,
there may be several possibilities in Ansys matching your needs, maybe one of the simplest is to set a Contact Sizing snippet so that only the faces belonging to the contact will be refined to the extent you want; for the rest of the solids, you could then set a rougher mesh. For problems which are "contact-driven", however, in order to get sufficient stability in the solution, the transition from surface to underlying material shall be "sufficiently progressive" and in effect one of the best methods to achieve this is through the Inflation like you have done. From your picture it only seems there is an exaggerated number of layers with, maybe, too small an expansion factor between one layer and the following.
Depending on the license level you have, also decomposing the objects into several different solids, and then using SpaceClaim to set congruent mesh at the interfaces between solids of the same component (group --> Shared Topology --> Share), may be of help: in this way, it is easier to exactly control the mesh size and progression, at the expense of bigger efforts in pre-processing...
Good luck, regards
- Badges
- Science topic