Tetrahedral mesh model under estimate the stress result

[Anonymous]

Hi,

I have done a simple circular solid cantilever beam and analysed with tetrahedral mesh in simulation mechanical. The result seems very less than the manually calculate stress result. But the brick mesh gives nearer results.

Can anyone help me sorting it out. I have attached the .arch.

Simple manual calculation.

Load - 1kN, Eccentricity - 300mm.

Section - 50mm diameter, Section modulus - 12271mm^3

Stress result = M/Z = 0.3kNm/12271mm^3 = 24.45 MPa

[John_Holtz]

Hi @Anonymous

The hand calculations are not calculating the von Mises stress. The hand calculations are for the bending stress. In the simulation, this is the "Stress > XX Tensor" results (because your beam axis is parallel to the X axis). These are the results from your models:

• brick elements: XX Tensor = -27.3 to +27.3
• tet elements: XX Tensor = -25.67 to +26.3

Both of these compare favorably with the hand calculation of +/- 24.45.

You should also try running the tet analysis using midside nodes (which is selected under the Element Definition).

The final difference between the hand calculation and the simulation is the constraints and Poisson's ratio. The hand calculation does not consider what happens when the "fixed end" is not free to expand and contract in the Y and Z direction. When the fixed end is fully fixed in the simulation, Poisson's ratio and the lack of expansion/contraction can affect the results. (With a square beam, you will normally see the highest stress is one node away from the fixed end.)  You might be able to eliminate these effects as follows:

• For this test model, set Poisson's ratio to 0. (You don't want to do that for a real model since it is changing other results.)
• Split the face on the fixed end into quarters. Then constrain the face and edges as shown in Figure 1. (Sorry that the axes in this old figure do you match the orientation of your model. )

Figure 1

[Anonymous]

Dear @John_Holtz

Thanks for your response. Before testing the simple model as you said, kindly find the attached 3D model(its a type of aluminium bracket for glazing). what type of mesh should i need to give for this type of model BRICK & TET or TET.

As per the attached model, i have given TET mesh type,

Von Mises Results :

TET (mid side node non included) = 195 MPa

TET (mid side node included) = around 345 MPa.

which of these results are correct, they is huge difference between the two, i got confused.

kindly help.

Thanks,

Giridharan S

[John_Holtz]

Hi @Anonymous

You should always use a brick mesh because it is more accurate.

Your mesh is rather coarse. Note how the stress goes from maximum to a small value over the distance of 1 element. That is an indication that the mesh is too coarse.

Because the maximum stress is one node away from a constraint, it is possible that the high magnitude is caused by a singularity. If this is the case, the stress will continue to rise as you refine the mesh. If it is not a singularity, the stress will level off at an accurate value as you refine the mesh. (You have a fillet of 0.5 mm radius. You probably want 4 or 5 elements on that fillet to capture an accurate result -- assuming the stress is not due to a singularity. That will give you an idea of what size mesh you will need to capture the stress concentration.)

See this article for more information: Why do stresses keep going up when the mesh is refined in Autodesk Simulation?