Learning Forum

[malbaro]

I would like to mesh the attached model such that the six contact reaction forces in the results must be equal. Currently, the model even after fine meshing at the contacts, the 6 reaction forces has small variation. 

Boundary Conditions are applied, Only one force is acting on the model. The main goal is to get all the six contact reactions equal. 

Thanks  

  

[Aniket]

Ansys staff can not download images or files on the student portal, so if you want to reach a larger audience to get answers from, please insert some images inline describing the problem.

-Aniket

How to access Ansys Online Help Document

How to show full resolution image

Guidelines on the Student Community

How to use Google to search within Ansys Student Community

 

[malbaro]

Done.

[Aniket]

This has been discussed previously on the forum. I haven't tried searching for the thread, but I would recommend you to search it.

Also, what is the variation in percentage?

Why do you want to equalize reactions?

Small differences can be observed due to numerical instabilities and it is very difficult to get results that are exactly matching for all the corners.

If you are sure that loading and model is symmetric can't you just model 1/3 rd of the model?

-Aniket

How to access Ansys Online Help Document

How to show full resolution image

Guidelines on the Student Community

How to use Google to search within Ansys Student Community

 

[malbaro]

Its not why but it should be. Logically thinking, if a force is acting on top face, the force gets equally transmitted to all the supports ( in this case 6 supporting balls). Which provides reaction forces and all MUST be equal. I am not getting all these reaction forces equal. it varies by +-0.01. I tried modelling 1/3rd model, in that case we wont be able to get all six contact forces in next analysis.(since all the six reaction forces will vary in next step)

[Aniket]

If you go on refining the mesh, while ensuring the mesh is exactly the same at all locations, then the difference should go on minimizing. When discretizing the model have you ensured exact same mesh? Also, what is "the percent" difference between reactions? Is 0.01 percent error? or absolute error?

Also, do you know about rounding off errors? 

https://mathworld.wolfram.com/RoundoffError.html

https://en.wikipedia.org/wiki/Double-precision_floating-point_format

The numerical error can still cause a difference in results even the mesh is exactly the same! One-third model will give you reactions and you can assume that the other two parts have the same reactions.

On a side note, there are many things in the world right now that MUST be equal, but still, here we are! 

[malbaro]

Hi Aniket, Thanks.

But as you go on refining the difference increases instead of decreasing. I mean the the difference between any two reaction forces increases. I was talking about theoritical model, where they must be equal. In ansys however they must be close enough and should not vary much but thats not the case. can you please check the attached archived file?  

[Aniket]

Sorry, Ansys employees are not able to (rather not allowed to) download any user files on the forum.

In reality, as well, there can be small differences, take an example of a perfectly manufactured cube of metal being released from a height, can you predict the impact point, edge or surface? Theoretically, it should always land on the bottom face, but in reality will it?

You did not answer my question. What is the percentage difference? tell us the difference between the minimum and the maximum reaction of the model?

Are you making sure that your mesh is periodic and exactly the same? Making that sure will not ensure that you will have exact same reactions, but it will reduce one variable in your model.

-Aniket

How to access Ansys Online Help Document

How to show full resolution image

Guidelines on the Student Community

How to use Google to search within Ansys Student Community

 

[malbaro]

 

I got why the reaction forces varies, as shown in the figure there is some sliding which occurs. Is there any way that the deformation occurs along the applied force as shown in the fig, which will distribute evenly and I think will get almost equal reaction forces if not equal.

[peteroznewman]

Hey Malbaro,

ANSYS uses a Force Convergence Tolerance of 0.5% to stop iterating. That is acceptable for most models.

If you want a smaller Force Convergence Tolerance, type in a smaller value, such as 0.01%

I recommend using a smaller tolerance for the Displacement tolerance also, like 100 times smaller.

You can also reduce the Contact Penetration tolerance.

After meshing, the geometry that was tangent now has small gaps of different sizes. When you use Adjust to Touch, that moves surfaces around differently for each of the six contacts. It would be better to move them all by a constant offset. I used an offset of 8.3e-4 mm which closed the 6 contacts.

Here is what I got with the above methods... +/- 0.0038 N

If you cut the three pins off the center body, you could mesh them with a regular swept mesh, which would reduce some of the variation. If you replaced the spheres with crossed cylinders, you would reduce the mesh variation even further.

[malbaro]

 

Thanks a lot, will try with your suggestions.

.

I had already got the required results without doing any of the above, Unfortunately I edited something and forgot to save the copy. Now I am wondering what I changed. Mathematical Result was 1.8190 and as you can see in above result it almost matches and not only that but it also satisfied all other boundary conditions. Only if I could get hold off that old copy.