Learning Forum

[deepesh.p.gurdasani]

I have taken a simple geomtery of a rectangular plate with 3 mm thickness (Fixed it like cantilever beam), and applied force of 10 N on other side. I get some equivalent stress. Now, after applying 'convergence' option, when it goes on refining the mesh, the stress increases with 40-50 % change upside. From what I know, with convergence, the stress should revolve around certain value or drop down until it becomes constant.

Is there any mistake that I am doing in the above procedure? 

Thanks in advance.

[peteroznewman]

Do some reading about Singularities. This is what you have in your model at the fixed support.  Take some courses about Singularities.

A singularity is a location of theoretically infinite stress. The peak stress in the model depends on the element size and keeps going up as the element size goes down.

Add a base plate to the fixed end of the cantilever beam, make it the same width as the beam and the plate extends above and below to make a T shape.  Add a blend radius at the two interior corners of the T equal to the beam thickness. Now you can put the Fixed support on the top of the T and the convergence option should show a line that flattens out.

[deepesh.p.gurdasani]

1) Thanks for the reply. I do understand about singularity and the recommendations given by you would possibly remove singularity but this would be changing the design. I would like to know wherever the singulairty occurs, is it possible to remove it by very minor to no design changes?

2) For using convergence option, should I mesh it with random meshing like just clicking RMB over mesh option and clicking generate mesh OR convergence would work even if I have already given size of 1 mm or something like that ?

Thanks in advance.

[peteroznewman]

A rectangular plate with a Fixed Support on the end face is not a real design, it is an idealization and simplification of a real design that is easy to analyze, but includes a singularity.

What is the real design? 

For a one piece part that is machined or cast, one real design is a base plate with mounting holes and a blend radius from the base plate to the integral cantilever arm. 

A different design might have a base part with tapped holes. A long flat plate with clearance holes goes on the base part and cantilevers off the edge. A short flat plate with clearance holes sits on top of the cantilever plate. Bolts clamp the long plate between the short plate and the base part. A detailed simulaton of these parts can create a model where the highest stress in the cantilever plate does not have a singularity.

Finally, you could have two fixed cylinders, one on the top side of the cantilever near one end and another one on the bottom side of the cantilever a short distance inward from the first cylinder. Use Frictional Contact between the cylinder and the cantilever plate. This method of support does not have a singularity.

[deepesh.p.gurdasani]

Thanks. got your point. 

1) Also, if any singularity occurs in the above design you mentioned (Assume a singularity occurs), is there any way to remove it ? any step by step guidance to try to remove it? like adding fillet or something like that.

2) suppose I get 50 Mpa stress without using convergence option and after using convergence option, I get to know that its a singularity, do I need to ignore this 50 M Pa as wrong value or it can be considered ?

Thanks

[peteroznewman]

1) For a design that has a sharp interior corner like the T shaped cantilever, adding a blend will remove the singularity.

2) If you have a singularity where the peak stress in the model occurs, the best option is to update the geometry to remove the singularity.  In some limited cases, you can use stress concentration factors or a web based calculator to calculate the peak stress from the geometry and the applied loads.