How To Cut Just The Outer Shape Of A Complex Component

[kencondal]

Suppose I've created a door lock as a component and it contains all the inner workings. I want to cut the outer shape of the lock from a door component so I can machine a recess to insert the lock. If I use Combine/Cut I get the (negative) inner workings left in the cut area.

I'm sure this is a common operation. What am I doing wrong?

Thanks,

Ken

[davebYYPCU]

Without seeing it or the file, I would

Copy the base door lock profile (sketch) if there was one, to the Door component, place it in position and extrude cut the door with it.

However I may have misread the problem.

[kencondal]

Hi Dave,

Thanks for the suggestion but I'm looking for a more generic solution (if possible). Sketches might not be available if the part was downloaded from McMaster or elsewhere.

What I'm trying to describe must be an incredibly common step that is used in design all the time. You have a bunch of components (bearings, motors, hinges, whatever) and another component (a housing) which must have pockets for containing those components. The pockets you need to cut only require the outer shape of the component (not it's internal details).

Take a trivial example where you have two cubes and want to nest the smaller cube in the larger cube (flush at the top, so the larger cube becomes a box without a lid). A Combine/Cut does this easily. But now suppose the smaller cube has a hole through its center. The Combine/Cut leaves a cylinder behind where the hole was. Sure, I could delete the cylinder left behind, but what if the inner cube had dozens of holes and other features? The 'simple' process now becomes extremely difficult and time consuming.

Since what I'm describing is done all the time in manufacturing design, there must be an easy way to accomplish this. I just don't know what it is.

What I want to cut is just a silhouette of the component, not its internal details.

Thanks,

Ken

[arnou-verfaillie]

@kencondal

You can try to make a new body/component with the boundary fill. These bodies/components can then also be selected to cut.

As done in the screencast below:

(Don't know why the combine/cut would not want to select the middle component, but selecting in the browser did it)

[HughesTooling]

I need to do this for mould design and your second example of a cube with lots of side hole is where Combin falls flat. Your only option is to build sketches\bodies from the part you want to cut out. Position the lock in the door create an offset plane on the face of the door and project the edges from the lock you need for the extrude cut.

Another option is to copy the body to another component and make it a solid you can use as a cutter, screencast I did for someone as a demo below. I have used software with auto core\cavity tools for jobs like this but they fail and would be just as much work for the part in the screencast.

Mark

[jeff_strater · Accepted solution]

Hi @kencondal,

I understand what you mean.  A similar problem is the "packaging" problem - you want to create some packaging for your product, say a foam block with a cutout that exactly matches your product.

There is no one-step way to do this in Fusion today.  We have discussed a "push" feature that would allow you to create such a cutout, but it's not on the radar just yet.

The one thing you can do is to use Sketch Project in the "Bodies" mode.  This does a silhouette projection of one body.  It won't satisfy all of your requirements, but I think it will get you close.

Here is a screencast, with audio, that shows the basics of this method:

Jeff

[kencondal]

Thank you all for the screencasts showing different methods for accomplishing this. It is now readily apparent that what should be a simple and common procedure, isn't.

I actually had used Jeff's method of projecting bodies, but as he mentions, if you have lots of bodies in the component (I do) it becomes extremely difficult to select all the right profiles and really doesn't solve the entire problem.

Hopefully someday there will be a "Silhouette Only" option added to the Combine dialog. Jeff, maybe you could add this to the wishlist of new features since you explain it much better than I do.

Thank you all for the suggestions,

Ken

[xnih13]

So, it is 5 years later, is there a built in feature to handle this today or is the silhouette option still the best option for this?