Using components to define a cavity - workflow question

[jandyman]

I'm starting to get the hang of components and assemblies, but there is something I want to do that I don't know how to approach, and it comes up often. I want to use the reusability of components to define cavities, after designing what goes in those cavities. Then I would import the component into another design in order to create the cavity in other bodies. The cavity shape therefore becomes reusable.

I've created a simple example that I've attached. It has an axle, a disk, and a "container" that has the desired cavity cut into it. The only purpose of this "container" component is to define the cavity. Then I want to go to another design and essentially import that cavity, maybe more than once, into that target design. 

I've come up with a workaround but it is very awkward. I create a giant body with the cavity in source component (bigger than the extent of the target body using the cavity), and import that into my target design. Then I have to position the imported body over the body that needs the cavity, and do a boolean intersect operation to get the cavity. It's very messy, and also the reusable component has to know how big the target body is in the design that is reusing the component. Is there a better way to do this?

My actual application has a much more complex cavity, and it is cut into both the top and bottom surfaces of the target body, which is in this case a bass guitar body. It's to implement a custom tuning assembly I designed. But I would use this cavity defining technique more frequently if it weren't so awkward

[davebYYPCU · Accepted solution]

I reviewed your file, 

What you said you want, is not what you did.

Why you modelled an axle and a wheel without a hole for the axle doesn't matter much, it's a demo.

Cut cavities with a cutter body.  You developed a sketch and 2 extrudes to do that at the end of the timeline.  Because the target body does not align with an origin, I used the Offset plane and Boundary Fill to make the cutter.  (There is no clearance for the axle.) 

This cutter is what should be saved out as a cavity cutter, for insert to new models, and then combine cut it from the target.

Might help...

[jandyman]

@davebYYPCU All your criticisms are fine, but like you said, it's just a demo, and I was aware of the issues. It's just to get the idea. 

I like your cutter body idea, and in this case it's easy because it is a simple cavity. But in the more complicated real life case, it becomes quickly complicated and non-intuitive. So maybe there is a way to create the cutter bodies from the complex cavities once they are complete, in the shared component file, by using a boolean operation? 

EDIT: Oh, now I see what boundary fill does, and maybe that will work as well. But if the cavity gets real complicated, then maybe the boolean idea would be easier. Experimenting now ..

[Drewpan]

Hi,

What you are asking is can I create a cutter using the real cavity a a mold. The answer is yes and it is fairly straight

forward operation and similar to what you have.

Take your actual cavity.

Create a simple sketch with a shape bigger than the cavity. Extrude the shape into a block.

Use a combine cut with the block being the body to cut the cavity body being the cutting tool.

What is left is a block in the shape of the cavity.

Save this a a component and use a your cutting tool for next time.

Cheers

Andrew

[davebYYPCU]

Not sure of your difficulty, 

if you can make the cavity, then making the void into a body is pretty simple job.

placing the cavities where you want them, maybe a little more difficult.  Joints and components make simple work of that.

Combine command is the Boolean operations in Fusion.

Might help...

[jeff_strater]

For either creating the reusable cutting component, or making the cut itself, try the relatively new "solid sweep", which allows you to select a solid as a "profile" instead of a sketch profile

[jandyman]

Yes, that's exactly what I mean by "boolean", and it does indeed work

@Drewpan 

[jandyman]

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@davebYYPCU wrote:

Not sure of your difficulty, 

if you can make the cavity, then making the void into a body is pretty simple job.

placing the cavities where you want them, maybe a little more difficult.  Joints and components make simple work of that.

Yes, I discovered quickly in experimenting yesterday that placing the cutter body where you want becomes the next issue. I figured it out for a simple part, but it may get messier for more complicated cases. If I can affix a joint to a sketch point in the included component (which sketch point may be outside the cutter body), that would be easy.

Still learning all this stuff in the component/assembly domain.