STATIC STRESS SIMULATION - DEFORMATION NONSENSE

[Anonymous]

Hi,

I made 2 spheres, took 1/8 of each of them an pressed one to the other.
I expected they will deform equally, with contact surface laying in the plane between them, but they don't.

only the initial contact point is where we could expect - in the middle between the centers.

Surounding volumes penetrated one into the another.

I put Automatic contact detecton with 2 mm contact detection tolerance, Separation contact type, asymmetric.

But result is the same if I put Symmetric.

What's wrong in my setup and how to correct it?

https://autode.sk/2ZVQWmF

[John_Holtz]

Hi @Anonymous 

It is difficult to know what is wrong with the setup by viewing a video. For example,

• what size are the sphere's?
• what size is the mesh?
• what deformation scale is being used to show the results?
• What are the material properties?

Here are some things that I see are not done properly:

1. The mesh is way, way, way, way, way too coarse for the contact problem. You should calculate the diameter of the contact region, and then use a mesh size about 1/3 to 1/10 of that size.
2. Contact is not a linear static problem. You should be using nonlinear static because of the "large displacement effects". As the parts deform, more nodes come into contact, and that is better captured with a nonlinear analysis.
3. In most simulations (and in virtually all linear simulations), the displacements are so small that they would never be visible if there were shown at actual scale. Therefore, the software exaggerates the displacements by some factor (probably 100's or 1000's of times the real life). My guess is that the video is not showing the actual deformation. For example, if there is a 1 mm gap between two points on the spheres, and if the displacement of those two points is 0.1 mm towards each other, and if the deformed shape is exaggerated by a factor of 100, it will appear that the two points move 10 mm and pass through each other. That is just a visual effect and due to not displaying the results properly. (Or not interpreting the results properly, depending on what you are trying to show.)

Let us know how the next analysis goes.

[Anonymous]

---

@John_Holtz wrote:

Hi @Anonymous 

It is difficult to know what is wrong with the setup by viewing a video. For example,

• what size are the sphere's?
• what size is the mesh?
• what deformation scale is being used to show the results?
• What are the material properties?

Here are some things that I see are not done properly:

1. The mesh is way, way, way, way, way too coarse for the contact problem. You should calculate the diameter of the contact region, and then use a mesh size about 1/3 to 1/10 of that size.
2. Contact is not a linear static problem. You should be using nonlinear static because of the "large displacement effects". As the parts deform, more nodes come into contact, and that is better captured with a nonlinear analysis.
3. In most simulations (and in virtually all linear simulations), the displacements are so small that they would never be visible if there were shown at actual scale. Therefore, the software exaggerates the displacements by some factor (probably 100's or 1000's of times the real life). My guess is that the video is not showing the actual deformation. For example, if there is a 1 mm gap between two points on the spheres, and if the displacement of those two points is 0.1 mm towards each other, and if the deformed shape is exaggerated by a factor of 100, it will appear that the two points move 10 mm and pass through each other. That is just a visual effect and due to not displaying the results properly. (Or not interpreting the results properly, depending on what you are trying to show.)

Let us know how the next analysis goes.

---

Thank You for your extensive reply.

Size of spheres is 20 mm in diameter, material is steel, max displacement is cca 0.005 mm (simulation result).
Size of the mesh - 10% of the part, minimum element size 20% of average, 10000 elemets, 16000 nodes .
I don't know deformation scale, but max displacement is 0.005 mm.

1. Adaptive Mesh Refinement was off in animation I have published. I turned it on in now, but result is similar: overlapping of the bodies still exists (in linear analysis), and I do not see any change in mesh density close to contact area.

2. I opened new, nonlinear simulation, assigned new, nonlinear stainless steel (from library) to the components, and put mesh size to cca 4% instead of 10%(but this is still much more than you suggested (did you mean elements to be 1/10 of real contact area, or 1/10 of contact area in adjusted representation?)  Now I can not find Adaptive Mesh Refinement option any more. Why?
Result is different, half of the contact area radius is shown let we say OK, no overlapping, but outer part of contact area is still overlapping.

3. I think I understand what do you mean, but - we have two surfaces (upper and lower) deformed some way - if we multiply their displacement by some factor (as we do in adjusted representation view) - the displacement of the surface points which are not in contact in real world should not be neither in contact  nor overlapped in adjusted (amplified) view, too.

So, let we use the amounts from your reply:

-initial distance between two points is 1 mm

- real displacement is 0.1 mm

- in adjusted representation Fusion multiplies it with 100

- both points will be displaced by 10 mm in displacement representation, but IN THE SAME DIRECTION, so  displayed distance between them should stay the same like in reality: 0.8 mm. Or I missed something?

You can access the file at https://a360.co/31yVFsd

[John_Holtz]

Hi @Anonymous 

Please review the documentation for the Deformation Scale. If you want your results to look realistic, you need to use the Actual scale. All of the "Adjusted" scales  magnify the real displacement by some factor so that you can see the motion. (Unless your vision is really good, you are not going to notice 0.007 mm displacement at an actual scale! 😁)

 

Here are the results at actual scale. Do these look correct?

Actual Deformation

These are the same results at adjusted "1x" scale. 1x does not mean 1 times the actual scale. It means 1 times the exaggerated scale that is used as the default. It is the same displacement, but the motion is exaggerated so that you can see what is moving. (Just eye-balling the results, the exaggerated magnification factor appears to be around 150 power.) 

Adjusted 1x deformationZero displacement at the contact point times 150 power = 0. 0.007 mm displacement times 150 power = 1 mm of apparent displacement.

About the mesh size. If you want accurate results, then you need multiple nodes over the contact area, not just 1 or 2 nodes. If I did my calculation correctly, the radius of contact is 0.18 mm. Therefore, the mesh size in the area of contact should be on the order of 0.06 mm or smaller. (One of the maximum stresses is some fraction of the contact radius below the surface. This is another reason to use a mesh size that is smaller than the contact radius.) If you do not need accurate stress and displacement, then a coarse mesh where potentially only 1 node is in contact is fine.

About the contact. I suggest that you use a Penetration Type of symmetric instead of unsymmetric. See Understanding master, slave, symmetric, and unsymmetric contact in a Simulation for more information about the differences.

Otherwise, the results are trending in the right direction! Let us know if you have any other questions.

[Anonymous]

Thanks, your answer and link about deformation scales helped me some way, but I have two more questions:

1. So, if I understood well, displacement of contact points  is shown based on origin of the system, but displacement of the points which are not in contact is shown based on the origin of their components? (that's why bodies overlaping?)

2. If I use nonlinear materials and analysis I can not use Adaptive Mesh Refinement, so to have precise results I should use very dense mesh in the whole components. Is there a possibility to split components in two parts: one close to the contact area and another the rest of the body, with different mesh elements sizes in these new, bonded components?

[John_Holtz · Accepted solution]

1. Your description is incorrect. The displacements are always relative to the constraints (which define the location of 0 displacement). It might help to look at only one component. The contact point (A in the figure below) deflects a small amount because of the contact. (If the upper sphere were rigid, the displacement at point A would be 0.) The rest of the sphere is deflecting twice as much (points B and C). Regardless of the displacement scale, the bulk of the sphere is displacing twice as much as the contact point. If you exaggerate the displacement scale enough, then it will look as if points B and C are "passing" point A, and then it appears as if the two bodies overlap. (And actually it looks as if the mesh turns "inside out" at the contact point.)
2. It would be better to split the face instead of splitting the body. Then add a local mesh control to the face to get the smaller mesh in the areas of interest. Splitting the body and using bonded contact adds an approximation to the analysis close to the area of interest (the contact point), so the bonded contact would have an effect on the analysis.

[Anonymous]

1. Oh, thanks a lot - I understand now!

2. But FEM is related to body (solid), so if I split only the face  - how will mesh be generated inside?

[John_Holtz]

True, the internal mesh might be a little better if you split the sphere into two parts and use a fine mesh on the entire tip part. (Better meaning a smaller mesh throughout the volume.) But I would rather have one part with no contact than have two parts with contact. The effect of the contact is worse than the effect of the mesh size (in my opinion).

I believe the internal mesh starts at the surface and works its way inward. So the size of the internal elements near the surface are close to the size of the surface mesh. Once you get "deep inside" the volume, you have no control over the internal mesh. If you cut the part and put a small mesh on the surface of a small volume, you will probably have small elements throughout the entire small volume. I think the difference is negligible compared to splitting the face and having small elements in a volume close to the surface and larger elements as the mesh goes deeper.

You can try it both ways and compare.

[Anonymous]

OK, but is it possible to set mesh setup differently for each body or face in system? How?

There is only one Mesh per Simulation Model in Browser (and many Studies per Simulation model), so it seems there is possible only one Mesh setup for all the components in Simulation Model.

[John_Holtz · Accepted solution]

Manage > Local Mesh Control.

[Anonymous]

Thx! 😉