## General Mechanical

#### Problem with convergence and singularity

• minko
Subscriber

Hi I have question about singularity and cnvergence.I have easy static structural problem. I have reactangle at one side fixe at second is applyied force. But I don´t uderstand convergence and singularities.

At the image you can see there are singularities at sharp corners but is possible to remove them? Or is some exact  way to say how exacty stress is? In hand calculation it shoud by 13 MPa but in sharp corners is 28 MPa. How i can say from this image how much stress is there?

I do some convergence but what this curve mean? It mean that it never convenge becouse there are singularities?

• peteroznewman
Subscriber

If you explain the supports and loads fully (or attach an archive), it will be easier to offer suggestions. For example, are those two edges selected to apply a force?  Applying a force to edges of a 3D solid results in a singularity because the theoretical stress is infinite since the area is zero. The solution is not infinite because the elements have a finite area, but as the elements are reduced in size, the stress increases without bound. If you put a convergence plot on those edges, the plot would just keep going up and never level off. Apply the force only to faces to avoid that.

Many times, a fixed support creates these kinds of stress concentrations that are undesirable. The stresses calculated are real. For example in a simple tensile test of a straight rectangular sample, the normal stress along the tension line cause a Poission's Ratio effect orthogonal to the tension line. At the clamps, a stress is generated due to that effect. That is why tensile test samples have the "dog bone" shape that flares out to a wider portion where the clamps hold the sample. Otherwise the straight sample would always fail at the clamps! This is not a singularity, and a convergence plot would show the stress leveling off. However, a hand calculation for a straight tensile test would not include the stress from the clamp, so if you are trying to compare an FEA result with a hand calculation, you have to have a way to ignore the elements near the stress concentration. One way to do that is with a multibody part. Slice your sample a little distance away from the clamp. Then plot the results on the body that does not have the fixed support on it.

Sometimes the geometry is symmetric. In the tensile test example, you can eliminate the stress concentration of the clamp by doing a quarter model. Slice the sample along the length, x, and through the thickness, z, and apply an x=0 and z=0 Displacement support on those two slice faces. Then instead of a fixed support on the clamp end, you can have a y=0 Displacement support. Now there is no constraint preventing the material at the clamp from moving in the y=0 plane and no stress concentration appears.

• minko
Subscriber

There is attached file look at it

• peteroznewman
Subscriber

The symmetry method delivers the hand calculation result.  The force has to be cut in half along with the geometry.

• minko
Subscriber

thanks