Learning Forum

[Franzanstein]

Hello!

I am currently doing different types of convergence studies but seem to be having a problem. Basically I am simulating a single spur gear in 2D (plane stress with thickness) using PLANE183 elements. The gear is held in place at the nodes of the inner diameter and a line load is applied along the flank of the studied tooth.

When doing a convergence study by refining the mesh of the tooth I get strange results. The Nodal displacement converges perfectly, but Nodal- and Element Von Mises stresses don't, as you can see in the attached graphs. Both start increasing in a bumpy way after an inital, small "convergence". In general the two values stay pretty close to each other. As you can see in the graphs the differences in the results between the first "convergence" and the last step are nothing extreme, but what could be a reason for the stresses not converging?

Details at location of max stress for step nr.7 (first "convergence") and step nr.20 (the last step of the convergence study) with visible mesh qualitiy:

[peteroznewman]

 

Displacement results always converge at a lower node count than stress results because stress is derived from displacements. The difference in displacement of adjacent nodes is used to compute element stress. Since each node has its own displacement error, the errors combine in the stress result, leading to a larger element stress error.

Are those nodal forces that you use on the flank?  A nodal force on the corner nodes of a quadratic element while midside nodes have zero force does not deliver a uniform pressure profile, but an oscillating pressure profile. I suggest you switch to PLANE182 elements to avoid this problem and use smaller elements.

Does the node on which the peak stress lands have a force on it or not?

Is the Stress Averaged or Unaveraged?

It is better to plot the element size of the elements in the vicinity of the peak stress rather than the node count of the whole model. Due to the way meshing is done, the element size in the vicinity of the peak stress might not change in proporortion to the total node count.

[Franzanstein]

Hi Peter! Thanks for the quick reply.

I rechecked the second example and it is a bit of a weird one so I’ll delete it and replace it with a different one. There is no force on the peak stress node, although the first node with an applied force isn’t too far away. I redid the simulation so that the forces are further away.

Yes I am using nodal forces, good point about the 182 elements, I had already tried both but there is very little difference, I’ll attach a graph where 183 and 182 elements are compared below but you can’t even see a difference: The convergence graphs are basically identical because the maximum stress is not close to the force application area.

 

 

[peteroznewman]

These are converging nicely, you just have to use smaller elements. In Mechanical, I would put an element Sizing mesh control on the tooth edge, while leaving the default element size constant. Then the elements along the front face edge can be small without incurring a large number of total nodes, since you don't need small elements on the back face, bottom face and top face of the tooth.