Hii folks, Today I was simulating the rubber and belt contact analysis. Maybe my contacts are not right. please check it and give any suggestion over it I am trying to simulate this.
here is the file
You should avoid applying boundary conditions within the contact regions.
Also, simplify the model for debugging. For example, you can skip the stationary pulley for now and analyze only half of the belt while making the rest rigid or removing it from the model:
rubber & roller contact non linear base displacement mod.pmx (1.1 MB)
I made some other adjustments/simplifications too. You should play with the contact stiffness because you have a large difference in the stiffnesses of both materials. You will find some tips here: Snap-fit contact snagging problem - Analysis issues - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
2 Likes
I can not open ur .pmx file so I’ can not comment on your set up, but I have attempted this sort of analysis in calculix before -I found it quite challenging! My best successes have been using membrane elements for the belt. I’ve attached a link to a video of one of my attempts
Thanks I will watch the video
Thanks a lot I will try it now
I got the point but I still not get how that belt is going to roll over the first roller and make the second roller roll
My suggestion is just to add complexity gradually as recommended - first get the contact between one roller and belt to work. Then if it’s working, add rotation (you could replace the boundary condition on a face with a rigid body constraint applied to the same face and enforce the rotation in the reference point of this rigid body constraint via BC):
You can add a second analysis step for the rotation.
Finally, add the second roller when the rest is working. You may still need to constrain the belt in the middle cut planes to avoid its rigid body motions.
1 Like
Ok got the steps, you mean I can get the contact between one roller and belt to work by adjusting the contact stiffness or just increasing value of displacement
Yes, that’s the best way to make it work. Usually, the default stiffness is too large. Apart from that, you can try refining the mesh while sticking to the rule that master surface should have a coarser mesh.
In the file I shared, contact seems to be working already, but I stopped the analyses without waiting until it runs to 100%. Maybe you don’t need to adjust the stiffness anymore - check how it behaves (and watch for too large penetrations with true scale deformation visualization in postprocessing).
Then the next thing to do is to reintroduce the skipped features such as friction, plasticity (although belts are usually treated as hyperelastic materials) and second roller - just make sure to add them one by one so that you know what makes it fail if it stops converging again.
OK got it, will sure do it