Can you use the same sketch for extrusions at multiple angles?

[DrCyanide]

I have a situation where I need to cut the same shaped slot out at different angles (0, 60, 120, 180). These slots are at different heights (based on different objects), so I can't use the pattern command to rotate the feature. 

Right now I'm creating 3 sketches that use the same parameters, one for the 0/180 degrees, one for the 60 degrees, and one for the 120 degrees. Is there any way I can use just one sketch to accomplish all of this instead?

[etfrench]

Put the sketch in a component by itself.  You can then Copy/Paste New the component and also place it with a joint.

p.s. You can also just put each of the slot geometries in one sketch and use a two direction Extrude (or From Object, To Object) to extrude each slot individually.

[DrCyanide]

Copying components to have copies of sketches instead of just having all the copies in the first component doesn't seem much better to me.

3D sketches will let me create the geometry all in the same sketch, and I can extrude them to the needed depths.

The problem with 3D sketches is that I can't seem to define sizes for the rotated geometry. For example, if I have a circle that I define as 5mm in diameter and then rotate it 60 degrees, Fusion 360 throws out the 5mm diameter definition. I can't re-add the dimension either, it won't select the edges of the rotated circle. Using parameters for the dimensions doesn't work either.

[davebYYPCU · Accepted solution]

In your case, 3d sketch has severe limitations, no profiles, no constraints, no dimensions, and very likely no parameters.

Stick to 2d sketches, you will at least get the job done.

Might help....

[DrCyanide]

Agreed. While it sucks to have a cluttered timeline and sketches folder, it's far more valuable to be able to change the dimensions later on than to use 3D sketches.

[etfrench]

A single 2d sketch works well although I think putting a sketch in a component is more flexible.

[DrCyanide]

I think you misunderstood my problem. I'll see if I can articulate it a little better (not able to use my computer with Fusion 360 at the moment).

In the X/Y plane I have the sketch of a hole. If you look at the X/Z plane you'll see several bodies arranged in a torus-like formation that I need to cut indents into, but NOT cut all the way through. I can use an extrude to make cuts above and below the sketch by using From Object, but I need a solution to "rotate" that cut to other angles. Circular Pattern won't work because I'm going to different bodies, which would make the resulting cuts too tall or too small. 

[HughesTooling]

You could extrude bodies then position with Move and use a Combine Cut to make the holes. That way you only have one sketch driving all bodies\cuts.

Mark

[etfrench]

A screenshot or drawing of this would make it understandable.

[DrCyanide]

The app has a good enough view for a screenshot to help this discussion. The large holes facing the center don't go all the way through the part, they only go a certain distance in. Each opposite set of holes were made using the same sketch, for 3 sketches total. The method worked, it was just a little tedious and left me with a lot of extra sketches and construction planes to align those sketches. I'm wondering if there's a method that would give less clutter.

@HughesTooling Combine Cut could work, but it would be tricky to align to the correct depth for each section. I wouldn't be able to use the current method I'm familiar with, which is Extrude From Object. Do you have any ideas what would help with the aligning?

[davebYYPCU]

In a previous thread, I remember suggesting making a cutter component, that had consistent cut detail, and the positions were not equidistant from centre.  

Place the cutter appropriately and Combine cuts to remove material, 

Did not work for you?

[DrCyanide]

That technique worked for some parts (the panels coming towards the camera are cut out using that method), but it didn't seem like a good fit for pieces that needed to be square/tangential to that curve. Towards the top of the screenshot you can see a rectangular cut out that will hold a nut, and below it you can see how the panel's connection curves away from it. 

[etfrench · Accepted solution]

Try it like this:

Each extrude cutter is a component put in position with a joint. Each cutter can be individually modified in the User Parameters or in their joint parameters without affecting the others.  There is one sketch to create the cutters and one to position them.

[DrCyanide]

I think that would indeed work for this kind of situation. I don't like that it creates so many components, but those can be Removed after use and I do like the flexibility of sliding the cutting head up and down. I'm sure I'll be redrawing this part in the future, and when I do I'll use this method.