Wrapping a body around a curved surface

[castleworksmotorsports]

In the attached file, I am trying to wrap the Firebird sketch around the top curved surface of the disc, and then machine that image into the disc at a constant depth (so that one part of the Firebird is not deeper than other parts as the contour of the disc changes)

I have tried several different methods by press / pulling the sketch into the disc then splitting the body, combining the two bodies etc....but each time the outer edges are shallower than the middle of the Firebird logo.

I appreciate any suggestions on how to accomplish this.

Thanks!

Kevin

[TrippyLighting]

If you're in the mood for an education thread that addresses that and then some, here it is.

[I_Forge_KC]

It's a dome @TrippyLighting 😉

Your error in the timeline aside, look what I did here...

It's not the exact form because I used your existing body to cut with. In a "perfect" world, you would loft from the bird to a point at the centroid of that sphere, then do the splitting and cutting.

[castleworksmotorsports]

I am pretty new to Fusion, so

Your result is what I am after, but I am not sure how you got there. Can you elaborate on the steps I should take doing it correctly from the beginning?

Also any input on the error I have (I am not sure what the error is) would be appreciated.

Thanks

Kevin

[davebYYPCU]

@I_Forge_KC quick today, 

@castleworksmotorsports you nearly had it, cut the bottom off, not the top, 

I used an offset surface for depth, you can change that, 

File attached, 

[TrippyLighting]

@I_Forge_KC Oops 😉

[castleworksmotorsports]

Thanks for all the input. It sounds like the steps I need to take are as follows

1. Press / Pull the sketch of the logo thru the top of the dome

2. Offset the surface of the dome down the distance I want the logo depth cut to

3. Cut the bottom of the logo off below the offset surface.

4. combine the bodies and I am good to machine.

[castleworksmotorsports]

So I am still struggling with this for some reason.

I tried to offset the face of the dome -0.050" and receive an error message (see attached screen shot)

I am selecting the top face of the dome, then selecting Press Pull, on that menu I am selecting "NEW Offset" as opposed to automatic and then entering in the value of the offset.

The error I receive is "The operation failed, try adjusting the values or change the input geometry"

[chrisplyler]

If you're going to mill this on a 5-axis then you will want to Loft the bird to the center point of the sphere that your domed top is part of. But attempting that locked up my computer, because your bird sketch is so, so awful. It's made up of like a gazillion little straight line segments. Horrendous!

Now I was able to just do a straight Extrude it, as you can see in the Screencast video below, but the geometry isn't going to be right for a straight cut endmill on a 5-axis. It's only going to be suitable for something like using a ball endmill on a 3-axis.

Anyway, here is an easy way to get the uniform depth using either scenario.

[davebYYPCU]

Your step 2, is in the Patch Workspace, 

Offset (surface body) for the cutter of the Split Body command.

Let me know if you want the embossing, normal to the dome.

I figure Lofting that sketch to a point ain’t gunna happen.

[TheCADWhisperer]

---

@chrisplyler wrote:

It's made up of like a gazillion little straight line segments. Horrendous!

---

I think either you are exaggerating or you misplaced a decimal point.

I only count 0.5 Gazillion.

[jasonhomrighaus]

that sketch is the issue  when I re drew it it lofted just fine.

What i did was simplified 1/2 of the sketch then lofted that to a point on a lower plane that matched the curve of the cap.

Then for some reason it didn't loft the cut outs so I lofted those out then mirrored the resulting body(much smoother was to do, complex sketches bog everything down)

I edited the Eye and Beak and lofted those in.

Next I duplicated the cap and offset it the depth of the Cut downwards and then hid it.

Positioned the Lofted bird on the cap and then combine cut it out.

Unhid the second cap and then merged all the bodies together.

the timeline is probably a bit messy but it should give you an idea of the work flow 

[castleworksmotorsports]

Can anyone explain why I got the error message that I did? Was I offsetting the face incorrectly?

Thanks

Kevin

[jasonhomrighaus · Accepted solution]

it had to do with the sketch.  There were so many points and at least a couple of little curlicues in the there that somewhere one of them caused the loft to try to turn inside out.  

I created a new sketch below yours and then projected points from your sketch to make a dot to dot that I could fill with straight lines and 3 point curves.  This radically simplified the sketch and made it loft friendly.

In this case its easier to set a Second body at the Height you want 

[castleworksmotorsports]

Thank you for all your work and the feedback. I am sure I Will be doing several other similar projects like this with different logos.

Kevin

[davebYYPCU]

This one has normal sides to the cut track, once I started I persevered. Could not make the outline work, in one go.

That Logo, was the cause of the problem, and similar source files will give similar hassles.

As @jasonhomrighaus found, a redraw to be more efficient to make Loft work,

I continued to Patch Offset, and lastly thicken the Patch bodies, and Combine Join them.

Looking closely, (tail feathers,) there are artifacts, arising from that sketch.

Might help....