topic Re: Creating channels on a surface - sweep not working for multiple paths in Fusion Design, Validate & Document Forum

Creating channels on a surface - sweep not working for multiple paths

micbond — Tue, 10 May 2022 16:25:57 GMT

Help,

I need to create a series of channels on a surface. A sweep using a cut with a profile connected to a path works for one channel. However the problem is that there are 20+ non connected channels (paths) and I want to use the same profile. Is there any easy way to do this other than repeating the profile, path & sweeps 20 times? This is an operation I will be doing regularly on projects so it would be great to find a much simpler way to achieve the same result.

Re: Creating channels on a surface - sweep not working for multiple paths

wmhazzard — Tue, 10 May 2022 17:00:10 GMT

Is each path the same? If so you could use a rectangular or circular pattern. If not please attach an f3d file of your model for better ideas.

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 07:02:36 GMT

here is an image showing one channel I have created using the sweep command, and several of the separate paths that I still need to create channels for.

Re: Creating channels on a surface - sweep not working for multiple paths

davebYYPCU — Wed, 11 May 2022 10:39:38 GMT

Round profile same size, use Pipe.

Path is same shape? doesn't look like it, (but pics not showing the details,) might use Pattern.

Might help......

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 10:43:01 GMT

Thank you for the advice, but I cannot use a pattern. Paths are always different but I want to use the same profile.

Re: Creating channels on a surface - sweep not working for multiple paths

davebYYPCU — Wed, 11 May 2022 10:50:31 GMT

Join the paths up with tangent semi circles, then it is one sweep. Top red line not literal.

Might help....

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 10:54:57 GMT

Interesting option. Then would you suggest I add fills in the red channels to remove these temporary features?

Re: Creating channels on a surface - sweep not working for multiple paths

TrippyLighting — Wed, 11 May 2022 11:13:48 GMT

I suggest you share your model. You appear to have yellow icons in your timeline. Fix those before continuing with anything else.

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 11:27:32 GMT

I have attached my Fusion360 model. Forgive my errors but I am an inexperienced CAD user.

Re: Creating channels on a surface - sweep not working for multiple paths

davebYYPCU — Wed, 11 May 2022 11:37:57 GMT

Now that I see what you want.

I would sweep or pipe cut these 5 in the quarter of the plate and mirror those features twice.

Might help....

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 11:40:59 GMT

OK, I can see how that would work. Thank you, I will give it a go.

Re: Creating channels on a surface - sweep not working for multiple paths

TrippyLighting — Wed, 11 May 2022 11:59:51 GMT

For this sort of design I would not use splines but lines and arcs as those are easier to capture and change with user parameters.

Then I would not mirror sketch objects, but timeline features.

Re: Creating channels on a surface - sweep not working for multiple paths

micbond — Wed, 11 May 2022 13:44:01 GMT

great advice. Thank you

Re: Creating channels on a surface - sweep not working for multiple paths

johnsonshiue — Thu, 12 May 2022 03:09:08 GMT

Hi! Instead of using Sweep feature to create individual bodies, you may want to use Thin Extrude. Here are the steps.

1) Extrude -> Type = Thin Extrude -> pick the individual splines -> set the appropriate directions and distances.

The splines will become solid bodies.

2) Fillet -> pick all the edges -> set the radius to half of the square length.

3) Combine -> pick the block as base -> pick the thin solid bodies -> operation = Cut.

The model is attached.

Many thanks!