Gear Stress Convergence

I'm working on the interaction between two gears to determinate the von Mises stresses on them. In order to make the simulation smaller I'm only dealing with a small piece of each gear, as picture below.

The contact surfaces on the teeth have been prescribed as frictional with a 0.1 value.

I'm using Revolute Joints to ground both gears, and in one of them I'm applying a 116 Nm torque and on the other one a rotation with zero value.

The standard element size is 3.8 mm, and I have parametrized the face sizing of the engaging teeth as input and the maximum stress on each gear as output.

And the maximum stresses location, with the results of a 2 mm face sizing.

This is the result so far, x axis is the element size (mm) and y axis is the stress (MPa). Gear 1 is the one with zero rotation, and gear 2 is the one with applied torque.

Any tips on getting the stress to converge?

Comments

  • @Cyberz

    Thank you for a well documented question.

    The geometry looks like it is sweepable. You should add a Mesh Method of Sweep. This will result in a mostly Hex element mesh. Hex elements are more efficient at filing the volume. When you sweep, identify a source face. Then apply the mesh sizing controls to the edges of that face.

    In a Mesh Refinement Study, it is more efficient to use a constant size factor to reduce element size. For example a factor of 1.5 would take you from a starting size of 2.0 in the following steps:

    It looks like the red curve for Gear 1 is starting to flatten out. With your new sweep mesh, start at 0.2 with the following sequence:

    Graph the data as you go on a chart with zero on the X axis. You don't have to do all the sizes down to the last one. When you have four points in an almost straight line, you can do a best fit curve through those points to extrapolate the stress to the zero element size.

    https://forum.ansys.com/discussion/538/how-much-mesh-refinement-should-i-do

  • Dear @peteroznewman , thanks for the feedback!

    Right now I'm not getting past the Sweep Method, and I get the "One or more non-sweepable bodies have sweep method controls and cannot be swept." error message.

    So my question would be, based on your experience, how should I slice/adjust the geometries in order to make them sweepable?

  • @Cyberz

    There is a circular arc on the flat face of the gear. Is the whole face flat or does that flat transition to a slight conical face on the ends of the gear teeth? If the whole face is flat, merge those two faces into one face. The radial cut faces have a split line that lines up with that circular arc. Merge the two faces on the radial cuts on each end and the same on the back side. Now there should be one face on one side and another on the other side. All the faces between the front and back face of the gear will have no split lines. That should make the geometry sweepable.

    Caution: CAD systems draw something that looks like gear teeth, but that is just a representation for space envelope planning. Real gears have a lot more detail than is represented in the automatically generated CAD "gear teeth". If you put the fully detailed gear geometry into the CAD system, you will get a more accurate estimate of tooth stress. The fake gear teeth that the CAD system created could have a stress results quite different from the real gear tooth geometry.

  • @peteroznewman you da man!

    Sweep Method worked as a charm.

    Got a nice convergence, although the stress values changed from my first series of simulations. I'd say that due to more regular hexa elements mesh the results are more accurate than the previous tetra mesh.

    Once again, thanks a lot!

Sign In or Register to comment.