Solved: Editing German Curve

Anonymous · ‎04-23-2019

Hi,

So I have this guitar model I am creating. Im trying to create a German curve that varies in size in various places.

I built a solid the created a pipe along the edge set to cut to create to the carve. It did what it should but it is a constant radius around the body. There are 4 sections where I need to modify the created body resulting in a non symmetrical carve.

The picture is a solid where I applied the pipe to create the carve (the top one was an experiment hence it doesn't go around the entire body).

Wherever there is an inward curve on the top path I want to move that inwards towards center, but I can't seem to figure out how I can do this.

chrisplyler · ‎04-23-2019

I'm not entirely sure I understand correctly, but what I'm hearing is that you would rather have an ellipse than a circle, and you would like to vary one dimension of the ellipse as it follows along the edge, such that it cuts more or less material away in different places along its path.

So instead of using the Pipe tool, make one new Sketch on the rear face and project in the edge so you can use it as a single, continuous path later. Then make a construction plane at each end of that path, and a few in various places along the path where you would like to define the various maximums or minimums of how much material gets cut away. Then a new Sketch on each of those planes so that you can define the appropriate ellipses. Finally, loft all the ellipses together in order and select the projected edge path as the center line.

Anonymous · ‎04-23-2019

Thank you!!!!!! I tried doing the follow rail method but getting things to line up exactly was a nightmare...your solution is exactly what I'm looking for and opens a world of possibilities.

chrisplyler · ‎04-23-2019

@Anonymous wrote:

...your solution is exactly what I'm looking for and opens a world of possibilities.

Oh good. I'm glad to help when I can.

Anonymous · ‎04-23-2019

Okay just got home and tried it...the ellipse worked kind of. I didn't like the look of the carve so I figured I could draw anything on the planes and loft them. So I tried a simple curve and got the dreaded "Would Intersect itself" error...which I understand but don't know how to fix?

Is there anyway to copy the shape from plane to plane? I need that reference to draw the next plane and it looks like Im going to need a lot more planes around the tight corners.

chrisplyler · ‎04-24-2019

The whole "would intersect itself" thing happens because you've got too wide of a profile attempting to turn around too sharp of a turn in the path. Since the profile always stays perpendicular to the path at any point along it, a turn that is too sharp will, of course, cause the inside bit of the profile to actually move backwards for a bit, and it will interfere with itself. Fusion 360 is not sophisticated to handle that math and produce a result anyway. The only way to fix it is to narrow the profile and/or reduce the tightness of the turns until that condition doesn't happen.

You can copy and paste sketch elements from one sketch into another sketch. But it isn't magically perfect. You'll have to project/intersect the path into the new sketch to get a point on which to make some sketch point (center of ellipse in my case) coincident with. It's almost easier just to draw a new ellipse for each one. If the sketch was more complicated, it becomes worth it I guess.

chrisplyler · ‎04-24-2019

This is the second time I'm attempting to post this. The forum ate my first attempt. It showed up, then I refreshed the page and it disappeared.

So...

You might want to take an additive Sweep approach instead of a subtractive Loft approach.

You'll want to define an outside and an inside body shape first, and make the base body with the base groove by two Extrudes. Then, if you Sweep a profile around using the Path-n-Guide-Rail option, you can use those two sketched shapes. If you use the interior shape as the path, then the profile cannot "intersect itself" right? And if you use the exterior shape as the guide rail, and use the Stretch setting, then the profile must always fit the varied width of the groove all the way around.

I used a Conic Curve, but you can use a regular arc or whatever. Note that I Projected/Intersected the two faces of the groove to build my profile on, so it must always adjust to fit the groove. Notice also that I fixed one error by adding some material to the profile such that it will positively Join the main body all the way around. You'll see that it took me a few attempts to get everything worked out correctly, but the result is as desired.

Using two splines to define the exterior and interior shapes does not lend itself easily to precision. For example, it's difficult to keep one spline exactly 1/2" away from the other spline for any continuous distance. I did an Offset of the outer spline and converted that to a construction line just so I would have a reference to eyeball. If you want a more precision approach instead of an eyeball approach, you would want to build the two shapes with arcs, lines, etc. that you could precisely dimension. If you do that, take special care to make all bits tangent to each other such that the Sweep can flow smoothly around.

chrisplyler · ‎04-24-2019

A link to the screencast above, just in case the forum doesn't display it like it should.

https://knowledge.autodesk.com/community/screencast/a985c601-c8c4-41cc-aa8d-653992d42921

Anonymous · ‎04-24-2019

Wow! Impressive! I can't thank you enough!

That looks exactly like what I am looking for.

I will be giving it a try...I will let you know how it comes out.

Anonymous · ‎04-28-2019

I simply cannot get it to work. I get all the same errors you do...but Im stuck where you first create what looks like a path extension (90 deg)...and then I have no idea where your orange hashed path came from... so obviously it never works. 😞

I also have a point in the top path so it is dividing it into two separate paths on the top object which might be causing issues.