How do I create constraints between components?

[MrGubbins]

I'm creating a U-shaped model which consists of a base and two sides. The sides are the same so after I sketch and create a component for one side, I "copy", "paste new", and position the second one in the correct place. My problem is that I don't know how to make the new component respect my user parameter dimensions.

For example, the base has a "BaseWidht" dimension and it adapts itself to the new dimensions as I change the value of my parameter. Trouble is if I make it bigger, the base adapts but the newly pasted side stays in the same exact position.

Is there a way to declare constraints against components just like you'd do inside a sketch so that I always know that my two "side" components always stay at "BaseWidth" distance?

[jeff_strater]

Hi @MrGubbins,

What are you trying to achieve here?  Are the two components going to be identical?  If so, then you don't want to use Paste New - this command creates a completely new copy of the component.  If what you are looking for is for the two components to be different, then use Paste New.  If you want identical copies, use just Paste - this creates a second instance of the component, which shares all the geometry with the first, so if you change that component, both instances will reflect those changes.

If you do want to use Paste New, then you will find a copy of every parameter in the original component.  For instance in the image below, I've used Paste New, and you can see that each feature, and the parameters for each feature have been copied, with an "_1" appended:

If you need more info than that, it's probably best to share your model.

Jeff

[Beyondforce · Accepted solution]

Hi @MrGubbins,

I just want to add to @jeff_strater post. You don't need to create a new sketch on the other side at all.

All you need, is to mirror your component to the other side and use the Joint to position them where you want them.

If it's not clear, share the file and we will show you.

Cheers / Ben
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[MrGubbins]

Thank you both for the prompt response. I think @Beyondforce hit the nail on the head when he talked about creating a joint. I'm learning Fusion 360 just for woodworking and hobby CNC machining and never thought I would ever need to do a joint but this suggestion makes sense. 

I'll play around with joints and pop back here if I need more help with this. 

Thanks!

[Beyondforce]

Great I'm glad it helped.
Fusion 360 is so easy to work with and the things you can do with it are remarkable. Now, I think because of it's simplicity, people tend to over complicate things.

If you have any question or doubt, just let us know.

Cheers/Ben

[MrGubbins]

OK, I thought I handled this but apparently I didn't! I'm trying to model a cajón drum which basically consists of four sides joined by rabbets on the top and bottom. The front and back are not included in the model to keep it simple. I'm including a file with a model I started from scratch with the bare minimum stuff I need to show this problem. 

Go to the Parameters panel and change a variable. You'll see that the box does not behave as expected; some components grow and move and others don't. I think the only one that works properly is the TotalDepth variable. The best reaction by far is when you change the MaterialThickness; things just rotate awkwardly. 

Any help is greatly appreciated. 

[jeff_strater]

Hi @MrGubbins,

I see the problem that you ran into.  It has to do with the fact that the components are joined with an As-Built Joint, which relies on the components being in the "right" position when the joint is created.  This can work if your components are created in such a way that, for example, the sketch is in the correct position.  This is the case for the first and second component in your design, but the instances of those components are positioned absolutely, not relative to the geometry.

So, instead, I'd use a "regular" joint to constrain the second instances of each side.

The screencast below has audio:

Good luck, and happy New Year!

Jeff

[daniel_lyall]

@MrGubbins Just for fun here is a different way to do the same thing, It's the way I do it as I find it a more stable way to do it with fusion and it is very user friendly way of doing it.

https://youtu.be/iQJMeBRq7G4

[Beyondforce]

Hi @MrGubbins,

@jeff_strater showed you how to create a connection between components with Joints. Now, I'll show you how to create connections with sketches:

Cheers / Ben
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[MrGubbins]

Wow, first of all, let me thank all you @jeff_strater, @daniel_lyall, and @Beyondforce for the incredible support. This is my first thread on this board and was not expecting this community to be this supportive. This is my very first project in Fusion 360 and the reason I'm learning it is because I'm building these cajon drums in my shop and it would be really helpful to be able to just change dimensions on the project and have the 2D plans magically update for when I need to build a different sized drum, which is very often. Currently, I'm doing this manually and it is very time consuming and the drums are a lot more involved than what I'm showing here in these models. Thanks to all your input I've learned a lot about how to go about and build this in many ways. 

Unfortunately, the only way that has worked perfectly for me is the one using sketches described by BeyondForce. My original way using components and joints still fails with what I think is a bug. Just in case this is still user error (and also while we are at it I might as well learn how to do the damned thing) here's a screencast of what I'm doing. The model is attached too.

[daniel_lyall]

@MrGubbins That's one for @jeff_strater I have seen that before, I cant rember What the problem is but it's easy to reproduces.

It makes it easier for the fusion guys to work out what is the problem, When you post the file and a screencast.

[jeff_strater]

The problem here is actually in your sketch.  It is constrained in such a way that multiple geometric configurations are valid solutions to the constraints, including the ones where the rabbet is backwards.  This is the problem sketch:

The way this geometry is constrained, particularly the equal constraints, this is also a valid solution:

 

[edit] - my first post had the wrong image above

Which is what happens when you decrease the TotalWidth parameter.

In general, you want your sketches to be as constrained as possible, to help prevent exactly this kind of geometry behavior.

Here is a screencast with audio explaining how to make this sketch more robust under edit:

Jeff

[MrGubbins]

Ah, I see! I didn't catch that the constraints were not strict enough! 

Again, thank you very much!