This is maybe a real effect, if stick slope is very sharp it can make snapping a bit bumpy, maybe Calc_em can do some tests in abaqus.
Thanks a lot. Can you share the .pmx file ? I implemented most of your changes and it works almost perfectly but the forces are too low. The devil is in the details so it would be nice to have a look at your setup.
Btw. the newest dev version of PrePoMax supports the *CONTROLS keyword.
OP also have tried different random models, so it’s not related to original geometry or not.
I can’t send pmx files sorry.
I see from your vid that there is still pending the smooth transition at the last step. That is the snap area and it is happening in a really short space. Mine has this amplitude.
Displacement value is set to 1mm.
Where are controls?. I can’t find them. Mine is a custom card.
By low force you mean in Fy or Fx?. I will take a look at that.
if original geometry still interesting, assumed material is Abs(default). Similar setup to previous: displacement control, hard contact, friction and rigid bodies apply. Quadratic tetrahedral element in use, mid-side nodes following geometry.
For me, it actually becomes worse with this amplitude and time increment of 0.005. I only don’t have *CONTROLS because it converges well:
Can you say or show how the block is constrained in your model ? Mine still has rigid body constraint but only at the top face.
It’s only available in 2.0.11 in a separate menu. I still use 2.0.0.
Both but mainly x.
Was it prepared in PrePoMax ? Can you share the file ? Did you check the forces ?
Now it looks just like in your model (setup should be the same, only without *CONTROLS):
but the force is too low. The maximum axial force needed to establish the connection should be around 3.3 N. In the model, the initial maximum is 2.29 N and then there’s a peak when it snaps back but I guess that it can be ignored.
Nice.!!
I guess it’s time to compare, look for discrepancies with given references and eventually improve the model.
I have reduced the clip run to the area of interest to speed up the results.
Regarding the peak I would consider:
-If you are comparing with analytical solution, Poisson ratio could make a difference. Your original set up was fixed and mine free to expand.
-The radius of the clip corner affects directly to the maximum axial load. The sharper, the more the clip must push down, the larger the normal pressure on the surface will be, the larger the friction force (nu*P), the larger the axial component.
-The recommended Stick Slope is 100 times less than the spring constant. It increases the axial force as there is a new tangential force involved. I have increase it up to the point it brakes the model. (80N/mm3). That’s is 1000 smaller. I think this parameter deserves it’s own post.
-The peak is still not smooth enough to isolate it. Maybe it’s time for some refinement.
For those asking why are we complicating the analysis of a clip in such a way with nonlinear and contacts . …In my case It’s just to understand better contacts. Jajajaj.
1 Like
it’s a general setup, no specific adjustment i did. Also, i’m interested in doing comparison with another FE solver, basic report can be helpful to understand a problem and the purpose of analysis.
below force outputs for my simplified examples, it seems sectional force is more appropriates instead of reaction.
I don’t mind this peak at the end so much as long as the initial forces are correct. I’m comparing them with Abaqus too.
What did you do to get this axial force around 3 N ? Only changed the stick slope ? When I set it to 80 N/mm3, it breaks the model, as you said.
But even 60 does it, the initial force is 2.9 N and then starts jumping incorrectly in the middle of an analysis.
My time period (1s) is now fully invested in a shorter run so it is advancing more slowly.
Note that the first elements to fail is a bad shaped Hexa.
That’s why I suggested to refine or work on the mesh. It has been very useful for debugging faster but now the mesh could be to raw.
By other hand I have also seen before models exploding when they are expanded with a unique element very large in depth.
Have you consider the corner radious geometry?
reduced mesh of original models: right side fixed, uplift forces. Even solvable, but still lack of interest since no other solver to be compared.
For now, I can use 10 N/mm^3 at most (this gives the axial force of 2.9 N so almost there). What’s your current value of the stick slope ? Refinement only makes it worse, like before. At some point, elements within the tip start collapsing (this is true scale, two subsequent frames):
I’ve tried various radiuses of the fillet on the block in the first tests.
I compare the results with Abaqus but only the axial force. It should be 3.3 N according to that solver.
these value’s for shear (uplift), axial force is about 1N (peak) reported by CalculiX
p.s rigid bodies apply at small block parts, hard contact with friction is left as original models
I have refine and use this final settings:
I have measured at both sides with identical results.3.1N
I think one should be carefull with the time step to avoid skipping the peak load transition.
Now that I have increase the time step from 0.005 to 0.01 seems like more springs disconnect randomly before time loosing their corresponding effect in Fx.
It’s being a nice example to look at. Let me know if you can give it a last improve.
1 Like
Sorry , I forgot to mention I changed Controls too.
*CONTROLS,PARAMETERS=CONTACT
0.001,0.1,10,170
If I understood properly this third parameter seems to control the stiffness relaxation. I was wondering how to limit the default reduction factor 100 . It has being my last attempt to remove those small jumps close to the transition but didn’t help.
That’s a very dense mesh. Mine looks like this now:
The initial max force is correct but there’s still this weird sudden behavior:
Actually, why is your amplitude 3.058 now ?
Mine is breaking too after the transition. I think that’s because slave becomes coarser than master.
I’m focusing on the area of interest.