I’ve created a sample part to look at how the test setup I create in PrePoMax changes the results. All cases have similar loading. (Question at the bottom)
The first has surface traction pulling “down” on the blue tabs to create tension in the part. The top ring is fixed (green)
The maximum stress happens at the root of the snap (green is over-the-limit).
I created a ring (shell mesh) that should do a similar job. It’s a rigid body, and fixed to a Reference Point. I use the same surface traction to load the part and have it pull against the immobile ring.
I can’t seem to get convergence using “contact”, so I created a contact pair as a tie, resulting in stress at the highest point of attachment. Not unexpected, but no realistic either. My use of the tie-contact on the vertical walls creates the problem
Instead of contact pairs, I created some Compression-Only constraints. The ring is still rigid and fixed, the surface traction is still the same.
This results in max-stress at the side-edges of the snaps.
Lastly, I tried to use the Displacement/Rotation constraints to describe how I expect this part to deflect. The green snaps have 0mm constrains in Y and Z and 0rad in rotX and rotY. This leaves them free to move and rotate inward - towards each other. To fully constrain the part I added the remaining two DoF to the green ring at the top: 0mm in X and 0rad in rotZ.
This created a stress distribution similar to the collar with compression-only constraints, but with a higher stress concentration. It’s hard to extend this thinking to other parts, but it works here because I have a symmetric part with axial loads. I just wanted to try it.
Which of these setups is the most realistic? What else should I have tried? I know FEA will confidently produce incorrect answers if I set up the problem poorly. I’m trying to improve my knowledge in that area. Any advice or reference material is appreciated.
A somewhat similar study I did recently: https://www.youtube.com/watch?v=yYuvUbu6Sw8
But I have a few comments about yours:
- non-convergence in the second case can be expected - displacement control should be used in place of load control whenever possible when dealing with contact
- use tied contact and check the contact pressure in the second case and you will see where contact acts and thus where BC would have to be located to give equivalent results
- compression-only constraint is not like regular contact pair - it doesn’t create an interaction between two parts/surfaces - it just creates a sort of contact with a virtual rigid wall to put it simply (and you don’t model that wall)
- nodes of solid elements don’t have rotational degrees of freedom so BCs applied to them have no effect
- it would be easier to model this when utilizing symmetry
- the most realistic setup should be the one with the fewest simplifications so the closest to the physical setup being modeled (like both lug and pin being modeled in my example)
1 Like
I took your advice exchanged the rigid shell for a 3D part made in the same material as the snap.
Contact pairs were successful with “Hard”. I have the same surface traction at the top, and the bottom surface of the collar is fixed.
I get a stress distribution similar to the rigid shell-collar, but with higher stress concentration.
All of this is just an exercise to improve my understanding of the tool and what user-errors I should avoid to make sure I’m getting the full use of the software
You could make that additional solid part rigid too (just for comparison). You have quite a few cases to compare (one could think about more but let’s not go too far). Now it’s a matter of accuracy vs time (spent on preprocessing and solving) ratio acceptable for you. Of course, simpler approaches are preferred, especially if you want to analyze multiple variants of this part.
I did as you suggested and changed only the one thing: I added a point and made the collar rigid (I selected the interior faces for the region - not sure if that matters). But I quickly got an error:
*ERROR in cascade: the DOF corresponding to
node 15 in direction 1 is detected on the
dependent side of a MPC and a SPC
Did you apply a boundary condition to the nodes involved in a rigid body constraint ? If yes, the boundary condition should be applied to the reference point instead.
That helped - the analysis runs
