Quick start for event simulation

[marc.liyanage]

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.

[henderh]

Edited: Please refer to Mike & Jeremy's replies below

[jeremy.wiesner · Accepted solution]

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:

1. Assign the appropriate material properties to your parts.
2. Apply a Structural Constraint to fix all three translational degrees of freedom (Ux, Uy and Uz) to the end of one part. I suggest fixing the two large faces on the right end on the large part. The gist is that you're going to want to fix one piece and move the other. 
3. Apply a Prescribed Translation to move the other part. I suggest applying the translation to the faces on the left end of the small part, which would be equivalent to pushing that part from the end. You'll need to specify a time-dependent translation using the Multiplier Curve in order to ramp the translation of the moving piece over the duration of the simulation. Let's assume you need to push the small part to the right 10mm, then you'd specify a multiplier curve that begins with a zero value at time zero and ramps linearly to a value of 10mm at the end of the simulation. The key here is to pick the appropriate duration for your simulation, and this may seem a bit counterintuitive at first. I'll give more guidance on this below. 
4. Enable contact between the two parts. Simply select the Global Contacts option in the ribbon and use the default options. You can specify a coefficient of friction in this dialog if you'd like, but I think you'll find that it won't make a significant difference if you parts are made of a smooth material like plastic.
5. Solve!

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.

[MikeSmell_ADSK]

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

[marc.liyanage]

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

[jeremy.wiesner]

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. 

[henderh]

Hi Marc,

Thank you for reporting the crash.  It's now logged in our system as ID ARRO-7035.

-Hugh

[marc.liyanage]

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.

[MikeSmell_ADSK]

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. 

http://forums.autodesk.com/t5/design-validate-document/getting-to-know-the-event-simulation-study-ty...

Keep us posted on your progress. 

Mike Smell

[marc.liyanage]

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?

[marc.liyanage]

Thanks Mike, I'll check it out. The URL is broken, I had to chop off "%C2%A0" at the end.

[MikeSmell_ADSK]

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

[jeremy.wiesner]

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?

[jeremy.wiesner]

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:

• Young's Modulus = 2.32 GPa
• Poisson's Ratio = 0.35
• Yield Strength = 30 MPa
• Ultimate Strength = 40 MPa
• Elongation = 30%

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. 

[marc.liyanage]

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.

[marc.liyanage]

Thanks! I'll try that material configuration next.

[jeremy.wiesner]

I'm glad to hear the most recent solve is looking better. I suspect there must have been something about the material properties that you entered that weren't quite right. If you can give me more details about what you entered and where I can help you figure out what went wrong. If you also point me to the datasheet you're referring to I can give you some guidance on how to setup a nonlinear material model for the Formlabs resin.

For plastics in general I think a deletion criteria of 0.05 is definitely more reasonable than 0.01. If you had a cast resin or a molded plastic, a much higher deletion criteria would be suitable, but considering your part is 3D printed I suspect it will fail at a much lower strain (though this is just a guess).

More often than not when running an Event Simulation study you will want to enable element deletion. The times when I would recommend turning it off are when you're confident that your simulation will not result in a part of your model breaking. Because you're not entirely sure whether the buckle will break, and you ultimately want to pull the buckle apart until it breaks, then using element deletion is definitely the right thing to do for this model. What you've observed so far is certainly not a normal pattern of element deletion, which looks to be caused by bad material properties. I think you'll find that the results using the acetal resin material are going to look a lot better!

[jeremy.wiesner]

I'm glad to hear the most recent solve is looking better. I suspect there must have been something about the material properties that you entered that weren't quite right. If you can give me more details about what you entered and where I can help you figure out what went wrong. If you also point me to the datasheet you're referring to I can give you some guidance on how to setup a nonlinear material model for the Formlabs resin.

For plastics in general I think a deletion criteria of 0.05 is definitely more reasonable than 0.01. If you had a cast resin or a molded plastic, a much higher deletion criteria would be suitable, but considering your part is 3D printed I suspect it will fail at a much lower strain (though this is just a guess).

More often than not when running an Event Simulation study you will want to enable element deletion. The times when I would recommend turning it off are when you're confident that your simulation will not result in a part of your model breaking. Because you're not entirely sure whether the buckle will break, and you ultimately want to pull the buckle apart until it breaks, then using element deletion is definitely the right thing to do for this model. What you've observed so far is certainly not a normal pattern of element deletion, which looks to be caused by bad material properties. I think you'll find that the results using the acetal resin material are going to look a lot better!

[marc.liyanage]

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

[marc.liyanage]

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.