In the November 9 2016 announcement (http://www.autodesk.com/products/fusion-360/blog/november-9-2016-update-whats-new-2/) the "Event Simulation Preview" was introduced, and it had an example of a buckle mechanism in action (see image below).
I want to do exactly the same for two snap-fit joints between two parts of a small case (see below as well).
I couldn't figure out how to reproduce that buckle simulation and I'd like to get a quick overview of how to set up the simulation to slide one of the two parts into the other and simulate the displacement and stress on the two snap fit levers. How do I go about that? I have the Ultimate subscription.
Solved! Go to Solution.
Solved by jeremy.wiesner. Go to Solution.
Edited: Please refer to Mike & Jeremy's replies below
Hi Marc,
I'm happy to help you get this model setup with an Event Simulation study. The simplest case would be to snap the parts together (without pulling them apart again). To accomplish this, you'd only need to do the following:
Now to talk about the simulation duration. The Event Simulation solver uses automatic time stepping, so you can't control how big each time step of the simulation is. The time step the solver calculates is chosen carefully such that the integration forward through time does so in a stable manner. The time step size is a function of the material properties (stiffness and density) of your parts, as well as the sizes of the elements in your mesh. In an ideal world, you would like to perform the snap-fit fast enough so that you get a solution in a reasonable amount of time, but not too fast such that the inertial effects of your parts moving through space do not influence the solution. For this model I suggest starting with a simulation duration of a couple milliseconds (0.002 or 0.003 seconds) and work from there. This may seem incredibly fast, but you'll be surprised how quickly objects structurally respond to loads. Given the detail of the geometry of your parts, I anticipate that a duration of 2 or 3 milliseconds will take around 25,000 time steps in order to complete the simulation. But don't despair! The time it takes to perform one time step using the Event Simulation solver is extremely quick. With a few iterations I anticipate you'll be able to achieve a good solution with this model that takes on the order of 20-30 minutes to solve.
Once you've successfully managed to get the parts to snap together, the next step is to pull them apart again. The only change you would make here is to modify the multiplier curve on your prescribed translation boundary condition. The multiplier curve should ramp the displacement up from zero to the amount needed to cause the initial snap-fit to occur, hold it constant for a short while, and then ramp it down to pull the pieces apart. Once you get here, this is when things start to get interesting. You can enable element deletion for your parts and specify a nonlinear stress-strain curve for the material. This would allow you to break the buckle when you pull it apart! This information can help you identify weak points in your design and quantify how much load the buckle can withstand before it fails.
Let me know how this goes and I can help you work through any issues that come up.
Hi Marc,
I will be glad to help you with this. Here are the general steps.
1. Enter the Simulation workspace and create a new Event Simulation study.
2. Define materials
3. Apply a Fixed boundary condition to the non-moving part.
4. Apply a Prescribed Translation to the moving part. Be sure to define the load curve to control the rate at which the moving part enters the non-moving part.
5. Click on the Global Contacts button to create the contact pairs.
6. Review the Settings under the Manage button on the toolbar to define your Event Duration.
7. Press solve.
I would also recommend looking at the Square Peg Round Hole Sample provided in the Simulation Samples > Event Simulation Samples folder.
Further, I will be putting out a forum post to provide additional detail and tips and tricks for using Event Simulation while in Tech Preview.
If you have any further questions, please let me know.
Thanks,
Mike Smell
Product Manager, Fusion 360, Simulation
Thanks Mike & Jeremy, that got me started, see video linked below, does that look right?
I need to play around with the material settings because the simulation shows the lever breaking off, but the actual 3d printed object behaves differently, nothing breaks there.
Note I also hit a crash (CER_139069951) when changing the step count in the Animate dialog to another value and then tabbing out of the field.
https://www.youtube.com/embed/38U_hFMiKG4?rel=0
Glad to see you got the model up and running! It's hard to tell from the animation, but it looks to like some elements are being deleted before the parts touch. Can you confirm if this is the case? Also, what do you have defined for the element deletion fields in the study settings (see below)? I suspect you have a value in the "Maximum Elemental Principal Strain for Deletion" that is too small. Assuming your 3D printed part is something like ABS plastic, a failure strain in the ballpark of 5% (0.05) is appropriate.
Hi Marc,
Thank you for reporting the crash. It's now logged in our system as ID ARRO-7035.
-Hugh
There is indeed something happening before the parts touch, I was wondering about that myself when I got the results. There are changes around the indents on the short part where the snap fit lever head rests in the final position. The edges in that area are changing even before the parts make contact. See the screenshots below of the first few frames with a close-up of that area. Is this what you meant with the deleted elements?
I'll re-run the simulation with the changed "Maximum Elemental Principal Strain" value that you suggested and report back.
Marc,
Glad to see you are making progress. As I mentioned earlier in the thread, I just completed another post on Getting to know Event Simulation. Be sure to check it out.
Keep us posted on your progress.
Mike Smell
BTW, I was wondering about another thing. When I hit the Solve button, the study, which I have set up according to your tips above, has the orange status dot instead of green, and the warning details dialog shown in the screenshot below lists a "No structural load defined" issue. Is there something missing in my setup?
Thanks Mike, I'll check it out. The URL is broken, I had to chop off "%C2%A0" at the end.
Marc,
This is just a warning. In your setup, you are using the Prescribed Translation, which is actually a constraint, rather than a load. Your setup is totally valid.
Mike
Yes, what you are seeing in those pictures are elements of your mesh being deleted from the model. This happens when you have element deletion enabled and the element is found to have exceeded the criteria you specified. This clearly isn't right, since the parts haven't even come into contact yet. There's two things I can think of that would cause this. First, if you put a really small number in the "Maximum Elemental Principal Strain for Deletion" field this could erroneously cause deletion to occur very early on. The other possibility is that your material properties aren't quite right. What material are you using? And did you override the default properties for that material?
Also, one other thing you may want to try. I recently put together a nonlinear material model for ABS plastic, which is attached below. The properties are as follows:
You can import this library into your Material Browser, at which point you can apply it to your simulation model. This would be a good starting point if you want to look at the failure of the buckle once the snap-fit is complete.
Thanks for the explanation Jeremy. Having element deletion enabled is the normal thing to do in this situation, right?
The value for "Maximum Elemental Principal Strain for Deletion" was at 0.01, and I re-ran it with 0.05 based on the tip above with better results.
I did fiddle with the material settings because I was trying to model the SLA printer resin I'm using (Formlabs "Clear" v2), based on their datasheet. It's possible that I got something wrong there, so I am currently re-running the simulation with a built-in material from Fusion 360's library (I picked "Acetal Resin, White" this time). That simulation is still running (each run takes about 1 hour) and I'll see if that material change, combined with the 0.05 value produces different results.
The change to 0.05 already changed the simulation result so that the snap fit lever no longer breaks off completely. However it's also not returning to the expected resting position at the end state because it still breaks a little bit on one side. The real-world material is more flexible and it deals with the amount of displacement of the lever just fine, but I'm not sure which value I have to change in the material configuration to get that into the model.
I'll see how the "Acetal Resin, White" material behaves.
Below is a screenshot of the material definition I made. It is based on this data sheet:
https://formlabs.com/media/upload/Clear-DataSheet_YgKm6wc.pdf
BTW, how can I import your material library into Fusion? I tried but I'm not sure if it worked. I have a material called "ABS Plastic", but its values are different from the ones you wrote up in the text of your comment.