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Sweeping a sketch
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Sweeping a sketch
I am currently drawing up my bridge design in Fusion 360. It has been a lot of fun and has gone really well so far. But I am a little stuck on rounding over the belly. I could easily put a fillet on it. But I want a little more round over on one side than the other. So I made a sketch on a plane of the curve I want to have. And then I try to sweep it across the belly, and it works, but it stops just shy of both ends where I want it to stop. There’s a push pull arrow but it won’t be pulled further. Is there a way to over ride that? If not, it seems like It need to make the line I am sweeping along longer. But I’m not sure how to go back and do that either.
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12 Replies
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I’ve never used Fusion 360 but, see if there is a way to change the radius on each end of the control curve you are trying to fillet. In Rhino there are handles that allow you to change the radius one each end or add handles to have multiple radii along a curve.
They can be finicky at the beginning or end depending on the radius entered.
Not sure if any of that relates to Fusion or not. It would be very interesting to hear how to solved the issue or what other people suggest. Customizing the radius of a fillet in this situation sounds easier than a Boolean nut that could certainly work too.
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This looks like a job for a Boolean cut. You know from doing that?
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Hey, you want to post the model you have so far? Looks like you can attach anything that is in a zip file.
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Here is a link to the fusion file. Please let me know if it works. I am very interested in hearing multiple ideas and i would like to try applying them myself so that i can learn something new. <div>
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I think if you were trying to sweep around that upper bridge line and hoping it will go passed the sharp corners, that’s a no go. I think you’d have to put planes at angles at those corners and then put sketches there and sweep those. Fusion wants a specific single line path to follow (I think).https://drive.google.com/file/d/1R2kgC6hlpvD2FpLvPhGTRpqcloUVO3iN/view?usp=drive_link
For some reason when I did the sweep on cut, it didn’t separate the bodies. So I couldn’t actually delete the waste part. Fusion sucks with little errors like that.
I was able to revolve the sketch around the front plane, but it’s not a consistent curve so probably not the look you’re looking for although it looks pretty nice I think. THere’s some shmutzy stuff right where your sketch is, not sure what’s going on there, could be a processing error, looks like 20 seconds of hand sanding to fix.
Just a strong suggestion: constrain your sketches as you go, either with dimensions or parameters. It makes a huge difference as your models get more complicated.
OK UPDATE
So the reason I couldn’t get the cut to work was because your belly radius profile didn’t intersect the top corner of your profile. So it was cutting, but it was cutting INSIDE the bridge, so the cut wasn’t visible. I lifted your profile up a tiny bit above the bridge so that it was fully overlapping the bridge and then I could do the cut.
I’m not sure exactly how you want to handle that sharp corner. If you’re looking to make those radiused also, you’ll need to do planes on those angles and add another profile there and sweep along.
THe other thing is if you want the sweep to go all the way to that corner, you’ll need a path that is on that bridge corner line but goes a little passed it. I think you could do that that with project include.
Let me know if that makes sense.
As far as constraining sketches, it would help you here. Basically you’re trying to connect everything to everything else. Your Belly radius sketch isn’t attached to anything, so it was missing the top of the bridge profile. If you had the bridge profile projected into that sketch, than the cut would work without adjustment.
It’s a really nice piece of work though, really good job.
Oh just another suggestion, for symmetrical shapes like this, mirror works really well. Then you only have to constrain one side and it keeps the dimensions to a minimum.
Hope that helps a bit.
First picture was the revolve, 2nd picture is the corrected sweep (with nasty nibs…that would be 2 seconds of sanding…)
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Actually tbh I don’t know how you could do a longer path on that bridge profile. Project include would just do what you already had.
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gotta say though, fillet looks pretty darn good.
One thing I’ve sort of excepted is that my design is going to change somewhat to make it CAD/CAM/CNCable. Stuff that might be hard by hand is super easy on CAD, stuff that is easy by hand can be very difficult on CNC.
So I’m ok with either
1) Leaving enough extra material to do handwork that would be really hard with CNC
2) Modifying my design a little to make it work well with CAD CAM CNC.
Just saying those sharp corners are going to be difficult. Not impossible. Also one way or another you’re going to have to go in with a chisel, can’t machine those angular corners with an end mill unless you get into some super hanky multi plane milling.
Fillet picture is attached.
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Is this what your were trying to do ?
https://youtu.be/Hgr8Fc_rLXw -
Ian! That video is above and beyond the call of duty! Thanks. Trying to defend that line was exactly what I was trying to do Monday. And I was trying to figure out what means of making a new plane to use. I will see if i can get that guy working now. If not, I may need a zoom call.
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Ok, I Got It!!!
First i moved the sketch 0.1mm up and out from the corner
Then i created a plane tangent to face and point. (secret ingredient)
Create a sketch in the plane.
Project 3d Geometry, Select top edge (where i went wrong…duh…)
Add small extention line of top edge. this will carry the sweep off the edge. (it was stopping just shy of the edge before)
Then sweep the sketch as normal, but selecting both lines to sweep along
Adjust sweep lenth as needed
Thanks so much again @ianhatesguitars as well as @PaulMcEvoyGuitars for taking time to help me. and paul, i am going back to sketches and adding constraints to further define them. Thanks for the tip. Maybe you can contribute some thought out information and experiences on constraints in an article sometime.
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Well for all my blathering, Ian fixed the problem.
It’s sort of hard to explain why constraining your sketches is so important until you start making more elaborate designs and having non-constrained sketches totally hoses you. I’ll try to make a little video about it if I can figure out a way of explaining it.
I think the basic thing is that if you are really, really good, and you’re nailing your design on the first try and you never want to modify it, constraining sketches becomes less important. And in this situation where you have an existing design you’re happy with, it is maybe slighly less important or noticeable.
But if you found you’d made a mistake along the way, or you wanted to do a 7 string bridge on the same design, or tweak a line or just generally experiment, when you go to change something you just have a bucket of random lines floating in space and you’re kinda screwed. Change one line and then you have to go down the line and change every other line because they aren’t really connected to each other. Usually though you’ll (I’ll) forget what I’ve done or why I did things a certain way and the whole thing is toasted.
Constrained sketches have a little red lock next to them. As you are making sketches, each one should ideally have the red lock. I’m not 100% on my designs but I really try to.
The weak point of constraints is the fix/unfix. The only thing you should use that for is for splines, which are hard or impossible to constrain. Occasionally I’ll use it if I can’t get something to constrain, but that’s weak on my part. It screws stuff up because it’s not really a constraint. Those parts can’t move.
there’s a command line in fusion and you can use it to find unconstrained elements in sketches. It’s very handy.
https://www.youtube.com/watch?v=matqB8nGzQIConstraints and the timeline also go together in a cool way. One of the great things about Fusion (no idea if it’s like this on other programs) is that you can slide back the timeline to an earlier part of your design, adjust something (like an extrude for instance) and then slide back on the timeline and the design should update, based on the stability of your design. Again, this is mostly for more elaborate designs with multiple bodies. This becomes hugely useful for modifying designs: say you wanted to put humbuckers in a strat for instance, you could slide back to where you extruded the pickup cavities, make a new sketch with humbuckers, extrude that, suppress the original pickups and then slide forward. If your design is stable, you’ll end up with what you want. Constraints are one way of making your design stable.
Anyway, I babbled again. I’ll try to make a video. Great job on the design.
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Here is an updated version of my bridge design for those interested. I started from scratch, because I wanted to make it taper toward the belly side to alleviate some mass. To do so I had to make a compound radius to maintain the wing thickness. Very interesting geometry. And it pushed my fusion skills to another level. Thanks again to my fusion helpers Ian and Paul.
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