Apply load in a specific area

[Max.H.Pour]

Hi guys,

I am having an issue with applying load on split areas:

1- When split surface is a rectangular and force is applied to it, I get 412 MPa maximum stress.

2-When I apply the same load into a split circle area instead of rectangular i get 692 Mpa

Both above methods, I sketch a 2D DWG first, then used project to surface tool to project it to 3D surface then split the surface into 2 parts that is where I got the circle and rectangular to apply the load into them.

3- This time I used 4 planes to limit the surface in a rectangular and the used split tool to split the surface. Therefore I get  more split surfaces which one of them is a rectangular where I want to apply load into. this time I get 432 Mpa.

So which one is more accurate and reliable?

Is it possible to use contact patches to apply load to?

[John_Holtz]

Hi maxhDL7VT

1. What type of load are you applying? If it is a pressure, then you need to be certain to adjust the magnitude if the area of the circle and rectangle are not the same.
2. Where is the maximum stress occurring? Is it at the location of the load? Is it just one node or distributed over several nodes?

My thought is that the mesh is too coarse. By changing the shape of the surface, you are getting a different mesh. Normally, results at small regions of loads or constraints are less accurate in simulation (FEA) and are usually ignored.

• If the area is really an area of concern, then you need to do several models and refine the mesh in each case. If the stress result stabilizes, then you know that you have "the real" result.
• If the stress continues to change, then you know that you have what is known as a "singularity" -- a mathematical situation in which the stress will continue to rise. Depending on the cause, you either need to extrapolate the result from nodes leading up to the concentration, or try a different way of modeling the load.

[Max.H.Pour]

Thanks John,

1- the load i am applying is The Force load. Actually the area of the circle and rectangular should be the same or slightly different, Circle with 10 mm diameter and rectangular of 100 sqm.

2-In most, the Maximum stress is happening in the area of load and it distributes over several nodes. Actually I refined the mesh in the load area for smaller sizes. This might be part of the issue?

[Max.H.Pour]

As I am using "Slice" command to create an specific area to apply load to, I am thinking maybe the slicing command is not appropriate for this model, The model is a Train Wheel and the forces must be applied to a certain area which in this case are presumed to be contact circle/Rectangular where the Wheels are sitting on rail.

[John_Holtz]

Since it is a Hertz contact type of problem, you can do a hand calculation to estimate what the stress should be. Then, in order to get close to that value in the analysis, you will need a really fine mesh around the load. My guess would be the mesh size needs to be on the order of 1 mm or smaller (but you can calculate that too with a hand calculation. The element size should be smaller than the depth where the maximum shear stress occurs.)

How the surface is split does not matter - whether you use slice planes to create the rectangular area, or sketch a rectangle and use the Split command. The only difference is the planes create additional surfaces which affects the mesh, but that is neither good nor bad.

[Max.H.Pour · Accepted solution]

Thanks for your help John. I have calculated the Hertzian stress and say its about 1110 MPa, to get the same/close results through FEA, I have rerun the Analysis for quite a few times. The only time I got the same/close results was when the mesh size is about 5.