Reaction force 0 when it shouldn't be

[Anonymous]

I ran an event sumulation on a bending test. The parts are a fixture (rigid), plate (polymer) and head (rigid). The head bends the plate 5 mm. I want to find the reaction force required to do this. However when I select the constraint at the head or at the bottom of the fixture I only get 0 N. I don't see what I am doing wrong. I created a similar model in ABAQUS and Solidworks Simulation and I was able to obtain the reaction forces there. Can someone tell me what I do wrong?

public link: https://a360.co/3srFSck

[shekar_sub · Accepted solution]

Hi, 

 

I tried to solve Study4 and the solve fails as shown. Maybe its a different study which you are able to solve?

We had some issues with reaction forces on rigid bodies and I believe it is the same issue that is in play here. That issue has been logged and I will add this dataset to that issue. 

Meanwhile if you could please let me know if its Study4 or some other study where you are seeing the issue would be helpful. Thanks

Regards

Shekar

[Anonymous]

Hi Shekar,

Thanks for your reply. I see that public link keeps track of the model changes. So unfortunately you have a newer version which does not include the old model. The study I ran was study 2. Study 4 has quadratic elements but i was not able to get it to work. 

I solved the missing reaction force problem by splitting the fixture at the bottom and make that part not rigid, but very stiff. This did give me the reaction forces I was looking for.

I have another question regarding the computational time. I did some research and found out that you are probable using an explicit solver for the quasi-static problems (see: https://knowledge.autodesk.com/support/inventor-nastran/learn-explore/caas/CloudHelp/cloudhelp/2021/... this is for inventor but i assume the same method is applied in fusion 360) . Since my model has a large boundary condition displacement, I assume the simulation time will be quite long. Combining this with the need for small time steps, due to the nature of explicit Time integration methods,  the simulation takes too long. I know that the time step size depends linearly on the element length, I used linear elements with a length of ~1 mm which did work. Then I tried quadratic elements. Since they have internal nodes on the edges, I assumed the element length should be ~2 mm. However the simulation time was still longer than 12 hours. Also increasing the element length even further did not work. Is my idea of multiplying the element length by 2 when switching from linear to quadratic elements correct, or do I miss something? 

Kind regards,

Chris

[Anonymous]

Hi,

Yes, there is a known problem in Fusion that it cannot recover the reaction forces on for the fixed boundary conditions on rigid bodies. Your solution to make the fixture deformable and fix nodes on the boundary (so their reaction forces can be recovered) is the correct approach.
Regarding the quasi-static solution procedure, it should be exactly what you want for this problem. In Event Sim, the automatic quasi-static procedure will automatically determine the appropriate duration for the event so that dynamic effects are negligible. That is, the inertial forces (mass x accelerations) are not significant. It does this by picking the largest duration for which the kinetic energy is a less than 2% of the internal energy in the simulation over a time averaged measure. There are a number of tricks used to perform this simulation including applying the loads with a very smooth "S-shaped" amplitude curve that insures there are no sudden jumps in the velocity. A trial and error approach is used where Event Simulation first uses a duration of something like 1000 times the initial stability limit. After it runs that initial guess for the duration, Event Sim evaluates the history of the energy balance and using a proprietary algorithm, it determines a multiple of that original duration that will give an essential quais-static solution. It throws away the original simulation and re-runs the simulation with this new duration. In almost all cases, this 2nd attempt is an acceptable quasi-static solution. However, Event Sim will apply the proprietary algorithm again and, if necessary, will compute a 3rd trial duration and re-run the problem. Running a 3rd trial is rare but will occur in problems that exhibit some kind of snap-through type behavior.
The automatic quasi-static solution gives you the shortest duration that generates essentially quai-static behavior. You do not have to put in a duration for the problem, we will figure it out and apply your specified displacement boundary conditions for you with an appropriate time dependent curve.

[Anonymous]

Hi Taylor,
Thanks for your response. I am (up to a certain level) aware of how the fusion 360 solver works. And I know I don't have to put in the time duration of the problem when doing a quasi-static analysis. However my problem is that the analysis takes to much time (more than 12 hours). I can't influence the total time length since this depends on the problem. So i can only try to influence the time steps. This is done by either changing the wavespeed (using a lower poisson's ratio or higher density material) or by changing the element length (larger elements). I try the second method, larger elements.
My question is, given that the simulation runs within 12 hours using linear elements of 1 mm. Should the simulation be able to solve within 12 hours when using quadratic(!) elements of 2 mm? This is what I assume, but it isn't what i observe. The Simulation isn't able to finish within 12 hours, or at least it predicts that it won't finish within 12 hours.