parametric pattern

[j2]

Hi Forum,

can you please help me?

My workflow problem is:

+ I´d like to create a number of joint-fingers with a user parameter. The idea is to create a solid to cut out the geometry from a block. -> Creating the geometry of the gap between the parts works fine.

+ But a pattern in sketch is no parametric step in the history -> doesn´t work

+ In the create dropdown the pattern function works, but then after changing the parameter for the number of fingers the number of bodies change and here breaks my workflow, because I have to chose the bodies for the combine-function manually -> parametric workflow broken

How is the appropriate concept in Fusion 360 to perform the task?

Thanks a lot ... Jörg

[lichtzeichenanlage]

This is the 2nd time today I've used the same technique. The first time was for pocket holes, this time for finger joints. Seems to be a reasonable technique to learn 😉

In my little experience with Fusion 360 I learned (by read threads in this forum and by testing several things) that it's often more reasonable to pattern features or faces and not use pattern in sketches. Reasonable in terms of performance and perhaps stability.

So I did a very simple finger joint and I'm able to create instances and to change more or less every parameter of each instance.

You can see what I did in this screencast, but it's not very straight forward, because I recorded by building the solution. So you can see all my fails 😉 In addition I've attached the design so you can play around with it.

[lichtzeichenanlage · Accepted solution]

For some reason the screencast was missing...

[lichtzeichenanlage]

@j2: 2nd thought about your post. Just because a single action (like a line in a sketch) is not directly visible in the timeline, it doesn't mean it's not parametric. Why? As long as the design changes by adjusting the parameters (user parameters, modle parameters) everything is fine. The timeline is useful. No doubt about that. But it's not the only tool in your toolbox. And if we want to be very precise - The sketch is part of the timeline...

[j2]

Hi Lichtzeichenanlage,

thank you for you post. So, the concept is to perform the task with feature.

Regards, Jörg

[lichtzeichenanlage]

Hi,

if it comes to patterns I would prefer features over sketches. And that's something most people would say here: Keep your sketches simple. 

I'm not sure if I understood your plan right and your plan is to use this component as a kind of cutting tool. If yes, I'm not sure if I would do this. But I'm a beginner. I would solve the task by defining a couple of components (positive/negativ join, negative/negative join etc.) and make those configurable. This might look like what I've proposed in this post:

https://forums.autodesk.com/t5/fusion-360-design-validate/pocket-holes-for-woodworking-drawings/m-p/...

[chrisplyler]

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@lichtzeichenanlagewrote:

@j2: 2nd thought about your post. Just because a single action (like a line in a sketch) is not directly visible in the timeline, it doesn't mean it's not parametric. Why? As long as the design changes by adjusting the parameters (user parameters, modle parameters) everything is fine. The timeline is useful. No doubt about that. But it's not the only tool in your toolbox. And if we want to be very precise - The sketch is part of the timeline...

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1. You CAN edit a sketch Pattern just as if it was an event on the timeline though. You get there by first selecting the Pattern constraint icon within the sketch and then right-clicking on it.

BUT...

2. Even if the sketch Pattern was set up with the number of elements as a User Parameter, it still won't parametrically solve correctly in a feature, once out of the sketch mode, because the feature (let's say it's an Extrude for our example here) must have had profiles selected, and when you update the parameter, which updates the number of patterned profiles in the sketch, that Extrude that follows the sketch on the timeline doesn't automatically know which if any of the new profiles you want to have included. You're going to have to edit the Extrude feature every time.

3. So the smartest way to handle such things is to sketch the intended feature ONCE, Extrude it, and then Pattern the Body it created. You can set up this pattern to use the User Parameter, and there isn't any guesswork that Fusion needs to do, because the profile(s) used as the basis of the Extrude isn't changing.

[lichtzeichenanlage]

i totally agree. And as I've written, I would prefer the feature based solution. But you can blow up a feature based design if you change the parameters, too. So that argument is valid but.. week. 

[laughingcreek]

I posted this in the other thread @j2 had going, but going to put it here to consolidate.

@lichtzeichenanlage, You can blow up any model by changing parameters if it's not carefully constructed.  but it's certainly do able.  see screen cast below made for a different user.

@j2-It appears i was incorrect about sketch patterns being a one shot deal(see @chrisplyler comments above), but it's still not a good idea to use a sketch pattern when you can use a 3d feature pattern, (as every body has said.)

[j2]

Thank you all very much for all the help. 

So, at a first step I changed the first part of my model to feature-based and it works. Well, I still have to clean up the overall concept a little.

Have a look: http://a360.co/2FXR48e

Regards, Jörg