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.

[jeremy.wiesner]

You can import the material library in the Materials Browser here:

Something seems strange about the screenshot of the material properties dialog you sent. The properties you entered look just fine. However, the base units are not consistent with the other materials in Fusion, and the Behavior option just above Young's Modulus line is an entry that I haven't seen in that location before. Is this material model from an old version of Fusion or from another Autodesk product? I'm wondering if there's a bug that is causing the material properties to not be written to the solver correctly.

I'll review the properties of the Formlabs resin tomorrow and help you put together nonlinear material models for both the green and postcured types.

[jeremy.wiesner]

I wanted to also provide some guidance for setting up a nonlinear material model for the Formlabs resin you provided the reference to. There are two classifications for the Formlabs clear resin: Green and Postcured. Here is the data the manufacturer provides:

Formlabs Clear Resin (Green)

• Young's Modulus = 1.6 GPa
• Tensile Strength = 38 MPa
• Elongation at Failure = 12%

Formlabs Clear Resin (Postcured)

• Young's Modulus = 2.8 GPa
• Tensile Strength = 65 MPa
• Elongation at Failure = 6.2%

In order to create a basic nonlinear material model, we need three additional pieces of data that the manufacturer did not provide: Poisson's ratio, density, and Ultimate Tensile Strength. But we can estimate these properties pretty easily. For Poisson's ratio I suggest searching online for what a typical value of Poisson's ratio is for resin. You can also search the Fusion 360 Material Library for a similar material to find missing data. From my search I think a value of 0.35 is reasonable for Poisson's ratio. I would suggest finding a density in much the same way. Based on my search, I think a number of about 1.2 g/cm^3 is a reasonable number. If you can't find the exact properties for your specific material, it's always a reasonable assumption to average data you find for similar materials. If you are unable to find the Ultimate Tensile Strength, you can use a conservative estimate for this number. The most conservative thing to do would be to use the tensile strength value (which would assume no strain hardening), but I think adding about a 10% increase to the tensile strength is very reasonable. If we fill in the missing data this is what we will use to create a nonlinear model:

Formlabs Clear Resin (Green)

• Young's Modulus = 1.6 GPa
• Poisson's Ratio = 0.35
• Density = 1.2 g/cm^3
• Tensile Strength = 38 MPa
• Ultimate Tensile Strength = 41.8 MPa
• Elongation at Failure = 12%

Formlabs Clear Resin (Postcured)

• Young's Modulus = 2.8 GPa
• Poisson's Ratio = 0.35
• Density = 1.2 g/cm^3
• Tensile Strength = 65 MPa
• Ultimate Tensile Strength = 71.5 MPa
• Elongation at Failure = 6.2%

To build the nonlinear material model, open the Material Browser in the Simulation workspace by clicking "Manage Physical Materials". The easiest thing to do is find the most similar material from the Fusion 360 Material Library and use it as a base for creating a new material. Enter "resin" in the search box in the top right of the dialog. Let's use the "Acetal Resin, White" as a base for the new material. So go ahead and double click this one to bring up its properties. 

If you click the "Physical" tab, you'll notice the material properties are greyed out. You can not edit the materials directly in the Fusion 360 Material Library. Click the button at the bottom that says "Add to Favorites & Edit". Now you can edit the properties and the name for this material which is now in your Favorites folder. On this tab enter Young's modulus, Poisson's ratio, density, yield strength and tensile strength. For the shear modulus, you can calculate this number from Young's modulus (E) and Poisson's Ratio (nu). The shear modulus, G, is equal to E/(2*(1+nu)). 

This completes the elastic material properties, but now we need to define the nonlinear stress-strain curve for this material. Click the "Nonlinear" check box in the top right corner of the Physical tab:

 

A new Nonlinear tab will appear where you can specify the data points for the stress-strain curve. You want to change the type to "Plastic" and use all the default options that populate below. Enter the yield strength for your material in the "Initial Stress Stress" field at the bottom of the dialog. The dialog will automatically populate the stress and strain value in the table corresponding to the point of first yield. For this simple nonlinear stress-strain curve, we'll only add one more data point at the ultimate tensile strength. In the white row of the table, enter the elongation strain and the ultimate tensile strength (in units of kPa). Your nonlinear properties should look like this for the Formlabs Clear Resin (Green). You can also click "Show XY Plot" to see the stress-strain curve as a plot.

Click Apply and the material will update in your Favorites folder. At this point you can right click the material, which is still named "Acetal Resin, White", and click Rename to give it the proper name. 

The material is now ready for use, so when you apply materials to your study you can find your new material and put it to use!

[marc.liyanage]

I *think* that I created this material by duplicating a built-in one, but I'm not 100% sure. Is there a way to start with a completely blank one?

I was able to import your materials library, thanks for the hint about how to do that. I re-ran the simulation. The lever still snaps off with this material definition, so I guess it's not a perfect fit for the Formlabs resin.

I'll re-run the simulation again but this time I'll disable element deletion to see how that turns out.

  

[marc.liyanage]

Our replies crossed, just saw your very detailed post about the custom material, thanks so much! I'll try this out, and I'll also contact the Formlabs people and ask them if they can update the data sheet with the missing information.

[jeremy.wiesner]

Hi Marc,

I'm glad to see you're continuing to make progress! I'm still surprised though that your model is breaking so easily. Are you able to share the Fusion (.f3d) file for this model? I would love to take a closer look at it and investigate what is happening.

[marc.liyanage]

Definitely, you should be able to get the model here: http://a360.co/2ekRtXM

Here you can see some photos of the printed object (some photos are out of date, I made the snap fit levers thicker later): http://www.thingiverse.com/thing:1839751

[marc.liyanage]

I just tried to create a material following your instructions, but my dialog looks different from yours after I copy the Acetal Resin, White material into my Favorites.

For one I don't have the "nonlinear" checkbox in the top right of the Physical tab, and I have that Behavior option that you mentioned earlier that is not present in your screenshot of the same dialog.

Is it possible that this is a Windows vs. Mac difference?

See screenshot:

[marc.liyanage]

By the way, even with the current results the simulation has already provided valuable insights.

For example, it showed me that because of the temporary deformation of the long part during the time when the snap fit joint is not yet fully engaged, the lugs that align the two parts collide in two spots, and I need to add some extra space there. That seems obvious, but I overlooked it since it's not visible in the perfect world of the regular model view. The simulation made it very clear.

[jeremy.wiesner]

It looks like the Mac version of Fusion has slightly different options in the Material Browser. I don't have access to a Mac, so @AndrewSears is going to look into this and get back to us. 

That's really great to hear that you're getting valuable feedback from your results so far! I've been working with your model for a little bit and want to provide you with some tips on how to get results a lot faster.

First, I converted your model into half-symmetry by deleting half the model. Since the geometry of the part is symmetric and the loading is symmetric, it is a common simulation strategy to decrease the runtime and still get the same information out. The basically approach is to split the model along the symmetry line and then apply frictionless constraints on all the newly exposed cut surfaces. The frictionless constraint enforces zero displacement normal to the surface (i.e. a roller constraint).

The next was to clean up the geometry a little bit to remove small features. Here is what the mesh originally looked like. Notice how the mesh becomes extremely refined in order to capture the small details, such as fillets.

I went through and deleted all the really small features around the buckle arm and the slot where the buckle snaps. I even changed the mesh settings to reduce the element size, and this is how the mesh looks now.

This improvement in the mesh is important for two reasons. First, we eliminated all the really tiny elements which means we have a lot fewer elements in the model. Fewer elements means faster runtime. We also are now using half-symmetry which means we cut the number of elements down further by a factor of two. But most importantly, we eliminated very small elements from the mesh that were causing the solver to use a very small time step size. The time step for this Event Simulation study is proportional to the smallest element in the model, so if we have even a single element in the model that is 10x smaller than all the rest of the elements, the time step would be 10x smaller as well. The result of this was that you needed 10x as many time steps to complete the same duration. By removing the small features from the geometry we've eliminated the really tiny elements that were controlling the time step size.

In addition to the above, I also applied the Formlabs Clear Resin (Green) material to the parts and I increased the deletion value to 12% strain (0.12) to match the elongation limit given by the manufacturer. The results looked much better around the buckle arm, but I also saw the behavior you described near the slot. 

The best part of this simplified simulation is that it only took about 12 minutes to get the results back. Much improved over the original simulation which took over an hour! I also wanted to mention that if you wanted to test the strength of the buckle once it's snapped together, in the mean time you could always try a simulation by beginning with the parts already pushed together. If you do this and then pull on half of the buckle, this would help you determine if there's any weak spots in the design that could be strengthened.

[marc.liyanage]

This is very helpful information, thanks again!

Two quick last questions about what you wrote:

1.) To apply those simplifications for the simulation, do you go back to the modeling environment and then delete the fillets etc. and slice the model in half? How do you do it so it's easy to get back to the unmodified model that will actually be printed (or milled etc.)? Do you just copy the entire design into a new project and run the simulation in there?

2.) Would it be possible to attach the adsklib file for the Formlabs resin that you configured, since I can't do it on the Mac right now?

[mcmillr]

You could go back to the modeling environment and  apply all the simplifications at the end of the timeline, then you can move your 'end of timeline' before the simplifications to get back to your original design. You just need to remember to do this when you are done with simulation. We are looking into other ways this can be handled for Sim users that will be more convenient.

Rob McMillan

Software Architect, Fusion Simulation

Autodesk

[jeremy.wiesner]

I second what Rob said about temporary workarounds if you need to modify your geometry for simulation. See below for a library with both of the Formlabs clear resins. I hope this helps!

[Anonymous]

A bit late to the party but this thread has been immensely helpful as I'm trying to do the exact same thing as @marc.liyanage but with Formlabs Flexible resin. @jeremy.wiesner is there any chance that you might have another file for the formlabs flexible resin that I can import into fusion?

Thank you!

Matt

[Anonymous]

Hi @Anonymous

Reviewing this thread, it looks like Jeremy created a custom library in Fusion with the data from the material data from the vendor. If you have the data for the resins you are trying to use, you can absolutely do the same thing pretty easily. Jeremy pointed out the key data required and the steps to do this. We have made a few tweaks to this workflow, see the latest help video on this topic - https://knowledge.autodesk.com/search-result/caas/screencast/Main/Details/d8a6945f-0688-411b-ae2f-862a96f84e20.html

If you follow this video and the details in this thread, you should be all set to get these materials into the Fusion 360 library and available for simulations. 

Thanks, 

Mike Smell

Product Manager, Fusion 360 - Simulation