CAM Engrave Text on a Curved (Not Cylindrical) Surface

[Mattfro91]

Hi all, I've been going insane over this for the last week. We have a 5-axis CNC and are trying to machine a sign with text and images around an outer ring. Engraving on flat surfaces is super easy, as well as cylinders, but I can't seem to make it work on even simple curved faces.

I've looked here, reddit, youtube, everywhere for an answer but I can't find anything that works. Not "Multi-Axis Contour", "Pencil", "Engrave", etc.

I need to be able to do the Engrave function where it stays within the boundaries of the letters and cleans up the corners, but stay perpendicular to the curved surface. I'm hoping I'm just missing something super obvious.

I'll attach the model that I'm working on. The shield in the middle is flat so I can do that no issue, but the letters and leaves around the frame I can't figure out.

Thanks for reading.

Losing my mind,

Matt

[evanp4509U4JZ]

Not sure how it would work in 5 axis but for similar situations 3 axis we use the "3D PROJECT" tool path. It maintains a depth of cut from the surface contours the sketch is projected to. 

I don't think it will make the depth of cut "normal" to a contoured surface but I'm not sure.

[Mattfro91]

I can see that being useful, and it would probably work if I was fine just outlining the letters and symbols instead of engraving them, and maybe I can convince the client to let me go that direction, but it's not the intended look. 😕

Definitely worth me keeping in my toolbelt though for future use, thanks! 🙂

[evanp4509U4JZ]

Does it need to be as deep as the model without the "curve cnc stock"? If so I think the only option is going to be laser it out of a .4xx" thick piece of material and then machine the curvature into the top surface. .438" deep with a cutter less than .063" diameter is an all day project with mediocre results that will have a cutter radius in all the corners. Send-cut-send or xometry could laser that out of 1/2" thick MDF or masonite if you don't have access to a laser then you could contour the top. 

Is it going to be a resin fill?

[programming2C78B]

you can cut the outline with the 3D path then remove the rest with a regular 2D pocket style operation.

[Mattfro91]

The final sign will be made from Walnut, then the engraved areas painted, then clearcoat everything.

When using the Engrave operation with a large chamfer bit the depth in the model doesn't matter since Fusion knows to just stay within the boundaries of the letter (or whatever), so you end up with a V-groove of varying depths as the tool moves up and down with both sides on the outer contours. I just model it deep so it has room to bottom out the tool in the toolpath; the v-groove only ends up around 1/4" deep.

Here's the toolpaths on a flat version of the sign:

It goes full depth in the wider areas but then pulls up where shallow or to clean up corners to make things sharp. You can see it on the engraved book here:

 

I just feel like there should be a "5-axis" checkbox for engrave to do this since they have the options for 3-axis and cylinders, but not other curved surfaces. 😞

 

[Mattfro91]

That might end up being what I have to do to power through this project, but it's not an ideal solution. I'm hoping to get this figured out though so at least the next time I get a client with a curved engraving I can confidently know how to do it correctly. There's gotta be a way to use the Engrave function for this if they have a way to do it on cylinders; it's such a powerful tool operation that it's a shame to have this limitation.

[programming2C78B]

The engrave toolpath has always been lackluster - you have to draw a fake boundary around letters to make it work for raised lettering! 

[HughesTooling]

If you can create a 3d body with the text extrude cut (no tapers) you can use Pencil to create a very similar toolpath to the one engrave creates. Used to use this before Fusion had the engrave op. Also used it on curved surface like you need.

[HughesTooling · Accepted solution]

Reading your post again I see the bit about keeping the tool perpendicular to the curved surface. Don't think you'll be able to do that but does it really matter as the cuts will be quite shallow.

This is what I get with pencil.

The calculation times seemed quite long so I copied the part and removed the centre leaving just the outer ring. File's attached, only did a small section. There was a rapid collision but you might get rid of that if you play with the Up/Down milling option.

[Mattfro91]

Oh my god.... you did it! I had seen the other threads mentioning Pencil but it just wouldn't work when I tried (and the processing times were dreadful). But yeah, it being perpendicular doesn't really matter with an engraving bit, but I figured it would be the right way to do it since that's what the Cylinder/Wrap version of Engrave does.

It's probably smart that you took out the middle section, that may be slowing it down as well; I'll just run the CNC in 2 operations. I'll have to see what was different between your Pencil operation and mine. I swear I tried so many variations with Pencil.

Thank you so much though!

[Mattfro91]

I literally can't find what was different from my original test models where I tried Pencil. I deleted the previous Pencil operation and replaced it with an identical one and it worked. Bruh, just a random generation error or something. But it works now! I'll take it!

 

[HughesTooling]

---

@Mattfro91 wrote:

I literally can't find what was different from my original test models where I tried Pencil. I deleted the previous Pencil operation and replaced it with an identical one and it worked. Bruh, just a random generation error or something. But it works now! I'll take it!

 

---

I've had ops that seem to go bad occasionally, usually when I've struggled to set something up and edited several times. Then create a new op and it works, compare and edit show both ops are the same but I guess there are some references to the model that have become corrupt or something!