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

[micbond]

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.

[wmhazzard]

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. 

[micbond]

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.

[davebYYPCU]

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......

[micbond]

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

[davebYYPCU]

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

Might help....

[micbond]

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

[TrippyLighting]

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

[micbond]

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

[davebYYPCU]

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....

[micbond]

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

[TrippyLighting]

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.

[micbond]

great advice. Thank you

[johnsonshiue]

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!