Bolt connections not being simulated

[Anonymous]

Hello,
I am trying to run a non-linear simulation of a box with a lid - the lid is held down to the box by a number of bolts. 
I set the contacts between the lid and the box to Free(as they are free to move if not bolted down since the lid "rests" on the box with a skirt around, like a shoe box) and set bolts to it around the perimeter. 
When I run the simulation with no preload to the bolts, and check Displacement results, the bolts remain stationary whilst the box and lid deform.  I am suspecting that the bolts are not being simulated.   Is this normal that the bolts do not move with the bodies during deformation, or not? 

I suspected this was because I did not add preload. When I tried to add a preload to the bolts, I get an error "Maximum number of bisections permitted reached".  
Am I doing something wrong?  Unfortunately I am not at liberty to share the model.  
Is there a tutorial/example of a simple box + lid + bolts I could follow, please? 

Thank you 🙂 

[John_Holtz]

Hi @Anonymous 

In your first simulation, the box and lid move together, as if connected by the bolts. Is that correct?

The bolts are just a graphics symbol, much like a force area is a graphics symbol. Neither the bolt nor force are shown on the displaced model. You should hide the bolts so that they do not cause confusion. (If I remember correctly, Fusion does not show the results in the bolts either, which are analyzed using beam elements. If they are shown, it would be a line along the centerline of the bolt.

In your second simulation with the bolt preload, you should change the contact from free to separation. (Actually, separation is the correct contact type for the first analysis, too. The lid and box can separate, but they cannot pass through each other. Free would allow them to pass through each other.)

Let us know what you find out.

[Anonymous]

Thank you for the reply!
Correct about the body parts moving together as if they are bolted - I thought that it might be just a bad representation however I wanted to be sure that that was the case, and not a bad set-up.

With regards to using Separation, when I tried using it the first time(without preload), I was getting an error(forgot exactly what it was), which is what led me to using Free in the first place. Tomorrow I will try to run the sim again with Separation set again and will try with and without preload and let you know.  We are yet to determine what preload, if any, to use that is why I want to keep it nil for now

Thank you once again!

Daniel

[Anonymous]

Hi again, this morning I tried to run it with separation contacts and preload and got this error: Insufficient Element Storage Space Allocated.  I added the error log below in case it might help. It says to increase the MAXADJEDGE, something I have no idea how to do.

If I leave the sim to free contacts(without preload) will it be accurate as well, or not at all since you said they would pass through each other? When I ran it with free they deformed together, didn't intersect though.

Thank you again 🙂 

[John_Holtz]

Hi Daniel,

Thanks for the log file. You will need to use separation contact in order to create a preload in the bolt. The analysis cannot generate any preload if the contact is free. (It would be like trying to tighten a nut when there is still a gap between the nut and washer.)

The error message indicates that there are too many contact elements. The only control that Fusion has to limit the number of contact elements is to specify the Maximum Activation Distance for each contact pair. Since the parts are bolted, I assume that they will not be sliding relative to each other. 🙂 Therefore, the activation distance just needs to be 1.1 to 1.2 times larger than the mesh size on the faces that contact.

I see one other thing in the log file. Your mesh is rather poor. The worst aspect ratio is 1.5E+5 because the longest edge (side of an element) is 0.161 m and the shortest side is 4.76E-7 m. (Wow, get out the microscope to see that one!) The ideal aspect ratio is 1. It looks like you either need a much finer mesh (before running the final analysis), or you need to remove the small feature that is causing the short edge.

Let us know if you have any other problems.

[Anonymous]

Thank you so much for the help! I managed to run it with preload and separation contact, I set the activation distance to automatically.  The results make much more sense now!

With regards to the mesh, I know it is very messy but I was more focused on trying to get the set-up right first before refining the mesh, so if I run a sim it wouldn't take long since chances were the sim wouldn't be correct anyways 😄  I tried to make it a little bit more uniform however I still have some very tiny sides which I cannot get rid of, at least for now. 

The last question - another sim I have been trying to do was an event simulation(to simulate the force as an impact over time - a rather big one of 35G over 60ms) however I was getting an error  that elements are detected with a negative volume that were not deleted from the model.  I tried to see intersections between the lid and bottom and there is none.  Could it be because the lid was created by taking a "counter shape" of the bottom, and not as a solid from scratch? 

Thanks! 

[John_Holtz]

Hi Daniel,

Good work on getting the analysis to complete by setting the activation distance to Automatic.

Good work on starting with a coarse mesh and planning to refine it later. Even after years of experience, it normally takes me a couple of runs to get the analysis to work like I intended (partly due to my errors, partly due to other issues.)

For the event simulation, the solution depends on when the negative volumes occur. The elements could start with a negative volume due to a poor mesh, or the elements could be crushed during the analysis and produce a negative volume (essentially breaking the elements). I am not sure if you can determine which one of those occurs; the output may not be specific enough if the analysis is failing. However, you can have the software remove the elements with negative volumes. "Manage > Element Deletion Criteria". If the negative volume is due to the mesh, those elements will be removed and the model has "holes" scattered throughout. (It is like a porous casting.) If the negative volume is due to the distortion, the elements are removed and the analysis continues. If enough elements are removed, then your model breaks apart and you see the pieces go flying.

[Anonymous]

Hi John,

Thank you for your feedback! So far everything is working great.

With regards to the event simulation, I did as you said and apparently it did solve something,  because now the sim is running beyond that initial negative body error. However now I got another error about energy balance calculation yielding an NaN quantity; I am attaching as a log as well(Error).  As Fusion said, and as I suspected, the load is slightly exaggerated.  I tried using the same load  over a distributed surface instead of concentrated, yet it resulted in the same result(Error 2)Just in case, is it possible that there is another problem other than the load magnitude, please?  

Daniel

[John_Holtz]

Hi,

I think the problem is related to the loads or the material properties, or the real part crushes beyond the capabilities of a simulation.

I think you are doing some type of impact. Is there a reason you are applying some type of force instead of simulating the impact? Is applying a gravity load (that is, an acceleration) more appropriate than a force load?

[Anonymous]

The simulation should be an impact/shock load of 35Gs for 60milliseconds - assuming that the housing plus it's contents(not included) weight 700kg total, I tried to simulate a load of 35Gs (700kg * 9.81m/s2 * 35) which is 240kN and lasting 60ms(0.06s in the time varying loading) acting on the side. I set the magnitude curve as in the screenshot. Does it make sense this way, or should I simulate it taking a different approach?  

[Anonymous]

I just figured I could have use a prescribed translation after some experimentation - which I believe suites my need better by using the actual acceleration caused by the shock impact over a period of time. I am trying it right now and will get back with the results. 

[Anonymous]

quick update, I set the prescribed translation as follows:

The result was 0 for anything. No displacement, no stresses, no reaction forces.  
I used 342m/s2 derived from the 35Gs of the 700kg. i.e. 240,000N/700kg = 342m/s2 = 9.81m/s2 * 35g

I applied this on one side surface, I fixed the opposite surface so it does not move with the force.  I am attaching a screen shot of the forces of a sample model.  The intention is to simulate a shock impact where the acceleration is put.  

It seems like I totally misunderstood the concept of prescribed translation

[Anonymous]

quick update, I set the prescribed translation as follows:

The result was 0 for anything. No displacement, no stresses, no reaction forces.  
I used 342m/s2 derived from the 35Gs of the 700kg. i.e. 240,000N/700kg = 342m/s2 = 9.81m/s2 * 35g

I applied this on one side surface, I fixed the opposite surface so it does not move with the force.  I am attaching a screen shot of the forces of a sample model.  The intention is to simulate a shock impact where the acceleration is put.  

It seems like I totally misunderstood the concept of prescribed translation and am at a loss of how to simulate what I need

[John_Holtz]

Hi @Anonymous 

At least you got results. That is further than some people get. 🙂

On a more serious note, your input looks okay. I did a simple test here to confirm that prescribe acceleration works, and it moved the model. I cannot think of anything that would be preventing it from working (as long as the part has mass and the same geometry with the prescribed motion is not constrained). There may be some clue in the output file ("Results > Inspect > Solver Data > Solver Output").

If you don't see anything obvious, feel free to export the model ("File > Export") and attach the .f3d file to the forum.

[Anonymous]

Hello John,

Apologies for the delay, I was away from home for a couple of days. 
Unfortunately I am not at liberty to share the exact model we are working on.
Would it be possible to upload a model of a plain box with similar conditions to how I set up the actual model, instead?

And just to clarify that I understood you well and we are on the same page, we are talking about an impact acceleration to simulate how an object would behave if it is hit from one side, and bolted from another(for example), not just how it would move freely, correct?

Kind Regards,
Daniel

[John_Holtz]

Hi @Anonymous 

If you can replicate the issue with another model that you can share, that would be great.

I believe we are on the same page. I applied a prescribe translation to a face and set the type to acceleration, just like shown in your image. To test some possibilities, I did two tests: one with a model and no constraints (so the body was free to move), and one test with a constraint on the opposite side from the acceleration (so the body would be stretched by the acceleration load).

[Anonymous]

Hello John,

Thank you so much for all your patience, really! 

So I tried it with a box(attaching the .f3d below) and it worked - same set-up.  I used lower acceleration since the box is smaller, and the fixed constrained points are slightly different too.
In the mean time I ran the simulation again with the original model and it yielded 0 stresses/displacements once again, which is very strange. 

Now I have deleted the old set-up and started anew.  However I noticed this time the sim is taking slightly longer, so it might actually be doing something(?), hoping for the best this time.

I would appreciate if you could tell me if my approach to setting up the test box is good to simulate a force over a period of time.  I will update you with the result of the current actual sim once it finishes too.

Kind Regards,
Daniel

[Anonymous]

Quick update, the actual sim now resulted once again in a NaN as before.  So I am assuming the fault is in the design not being able to withstand the set load.  Although it does seem strange - for the box I used only 1/2 of the acceleration but it has thinner walls and no inner structure so should also be much weaker.

[John_Holtz]

Hi,

I took a look at the test box. The only thing that I see is that the total event duration is set to the default (0.001 sec) but the prescribed acceleration curve is set to 0.18 sec. The analysis may run, but it only covers a very small fraction of the total analysis. (I tried running it with a total duration of 0.18 seconds but stopped it after 3 hours. With a duration of 0.001 sec, the analysis completes in under 1 minute. The time step size of 1.44E-7 implies that 0.18/1.44E-7 = 1.25 million time steps would need to be solved to get to the full duration, and that is why the analysis takes a long time to run. I see that plasticity is activated, so the time step will get smaller (more calculation steps and longer runtime!) if the part begins to yield.)

For the question of whether the load is a good representation of the real situation, that depends on what the real situation is. If you have a specification that says to test it for an acceleration for a certain rate, you need to duplicate what the specification means as far as where the acceleration is applied, the ramp, and so on. If you are simulating a drop test (whether dropping the box or dropping something onto the box), then that test can be setup in the event simulation.

[Anonymous]

Aha, so that is what I was not getting at all, I assumed that the event duration would automatically be set to the duration of the prescriber translation!  And no deformation was occurring because the acceleration was set to start at 0.06s, well after the event duration ends. 

Now I extended the event duration(to 0.06s, and set the acceleration to be applied from 0 to 0.06s) but it is returning an error whenever I try to run the sim as attached in the log file.   The sim is failing almost instantly.  No specific error, just that it could not be solved.  I checked the error log myself, and I saw that it could be due to the duration time set too long(I doubt 60milliseconds would be considered too long).

Again, I adjusted the test box I had sent you, set the event duration to match the one for my model and so far it is running with no issues, at least it has been running for much longer than the other before it returned the error.   Once again I am at a loss, to see two same set-ups behaving differently/returning different errors.  

With regards to what I am after with this is basically to simulate a box(that houses a component in a vehicle) for an impact shock - one requirement is, for instance, 25G for 60milliseconds half sine (there are various ones though).  I decided to constrain the side opposite to where the acceleration is applied because I took the assumption that the box cannot move there since it will be held in place by the vehicle - not going into the detail of how the vehicle itself would behave on that end.