Simulation, problem of constraint singularities

Simulation Generality
1

Hello

I have a simulation problem with my part (crankshaft).

When I refine my mesh in my part, the stresses diverge because of the stress singularities detected at the sharp edges.

If I add fillet to the sharp edges and round the corners where high stress gradients occur, how much radius I want to choose for those fillets...because the stress varies wildly depending on that radius!

Are there other methods for this type of singularity problem?

You will find attached the document with an explanatory diagram.

I hope you can help me.


190319--vilebrequin.rar
2

Hello@calcul

I will look at your document to verify that you are indeed in the case of constraint singularities and not in the presence of legitimate concentrations of constraints.

I will keep you informed as soon as possible

Kind regards

3

Hello@calcul

I have looked at your simulation and I do not see any singularity of constraints.

On the other hand, what I see

  1. It's that your mesh is too coarse, which means that you make max constraints appear where in fact there are none.
  2. Once a mesh is finer in the MIN values, you arrive at a Von Mises value of 64 for an elastic limit of 235 and moreover no abnormal stress concentration.

In short, your simulation is totally wrong and only serves to falsely reassure you. Especially since remember a previous question where I pointed out that the two weak points were the welds at the crankshaft and possibly an excessive twisting of the shaft in its longest part. As luck would have it, your simulation doesn't take these two elements into account either

Kind regards

PS: On the other hand, I think that you would still be better off seeing the person who trained you on SW simulation because I am absolutely sorry to tell you this in such an abrupt way because it is not in the spirit of the forum  but your simulation as it appears to me in your last file is a complete nonsense. I am referring here to your imposed travel. Ask yourself why you don't use pivot stress or bearing load.
There is also a big inconsistency in relation to the function of the small tree (the short one). Generally speaking, I suggest you review the connectors such as shafts, bearings, solder beads and for loads the usefulness of "torque" for example.

4

Hello Mr. Zozo

1/ Maybe I wasn't precise about my question!

In the first step, the objective is determined the MAX stress in these 3 bodies (Main crankshaft axis/webs/Crankpin). You will find attached more details on the definitions of these 3 bodies. For the record, the 3 bodies are welded together (that's why I don't use pivot or bearing load constraints, axle-type connectors...

Then, I calculate the stress in the weld seams using the 3 Von Mises MAX values obtained (by SolidWorks) on these 3 bodies of my model. I was forced to go through this method because SolidWorks does not allow to make a stress calculation, while respecting the given standard, on these weld seams. That's why I don't model weld seams!

To be much simpler and faster (12 simulations to do: the loads are rotated every 30° to consider all the possibilities), I tried to model my beam part. But the problem with this modeling (in beams), I can't run a fatigue test.

2/ I don't get the same result as you! I don't see how you got the Von Mises value of 64 MPa without an abnormal stress concentration while keeping the same load and displacements imposed!? Can you tell me the MIN element size and MAX element size values you took?

Have you tried refining the mesh even more to see if the MAX value of Von Mises converges or diverges? We cannot conclude from a single calculation (even with a single fine mesh) whether there are indeed singularities of constraints or not!

-> The "stress sensitive points" tool indicates that there are stress sensitive points (attachment)!

 

In my case, and with a fine mesh, I get a value that varies between 64-77 MPa, far from the 64 MPa you obtained:

- 67 MPa for a mesh (MAX element size = 10 mm and MIN element size = 2 mm).

- 77 MPa for a mesh (MAX element size = 5 mm and MIN element size = 1 mm).

- 68.8 MPa for a mesh (MAX element size = 2 mm and MIN element size = 0.4 mm).

 

In addition, when I try to refine the mesh at the constraint-sensitive stops, I get stress values that start to diverge (see attachment). This is normal!

I come back to my questions:

-Is there a method for this type of "stress sensitive points" problem?

-I want to stop at what mesh size to see a reasonable result ? And why?

 

Kind regards.

 


points_sensibles_de_contrainte.pdf
5

Hello @calcul

You are only in the presence of false sensitive points of constraints for the following reasons.

 

You don't respect the sacrosanct rules of simulation, which dictates that you always use a simplified model. This means that, for example, as in your case, you have a mini chamfer (like deburring) which alone generates a false sensitive point. A simulation is always done before the model used to make the MEP, which means that it is simplified as much as possible by removing all the chamfers, fillets, useless, etc.

Same for the H7 and C° game

Remove the mini deburring chamfer and your sensitive spot will disappear !

You should always be wary of red areas in simulation, especially if you show it to the chef or a customer.

Here are some additional pieces of evidence on what I am saying.

  1. You have a Von Mises that is one-third of the elasticity limit. This shows that from the point of view of solidity you are far from the limit.
  2. If you set a graph of the safety factor with a limit greater than 5, you will realize that you are everywhere with a coefficient greater than three
  3. If you look at other places you also have false positives (on the long tree where you have areas that I assume are supporting).
  4. The places where you don't have the deburring chamfers, you don't have artifacts and therefore no hot spots.
  5. From the point of view of design choices, you have no fillet in the corners, which automatically generates stress concentrations. It's not a big deal , but it can also generate false positives. If your parts were fretted, you wouldn't have its false positives either, at least as long as you have the limited efforts you indicate. It will be in your best interest to have a very tight assembly.

That said, it's a shame that you didn't give me the real parts but only parts imported from I don't know where: because I would have shown you another way to do the simulation closer to reality, especially on the twisting of the long portion of the shaft.

Kind regards


presence_de_fausses_singularites_de_contraintes_.pdf
1 Like