Switching side engraving tool engraves on of a line

[jfrankovich]

Hello!
I am trying to use the engraving tool with a 90-degree vbit to engrave a design onto something. However, engraving traces out the inside line of my design rather than the outside line. Is there a way to change on which line the engraving mills? 
I'm sure there's some obvious method, but I can't find it.

In my screenshot, you can see a circle engraving onto a block, but the engraving is on the circle's inner edge rather than the outer edge.

 

[hyperbolicindustries]

When selecting the line in the operation, you should see a red arrow. Click that to change what side the operation is cutting on.

[jfrankovich]

 Forgive me im not sure i understand. I don't see a red arrow* to select

[jfrankovich]

I want to do similar to around 12:20 in this video Beginners guide to vbit relief carving - fusion 360 90deg v bit Workbee cnc - YouTube
but instead of cutting the outside edge, it cuts the inner edge 

 

 

[hyperbolicindustries]

Can you File>Export>*.f3d and attach your file.

[hyperbolicindustries]

And I think you are a little confused between using [Engrave] which varies its height based on the distance between the 2 driving lines/curves and something like [2D contour] or [Trace] which is just driven by the line/curve section.

In your example video the [Engrave] is being controlled by the outside circle (which is just curves because its broken and not a closed shape) and the outer edge of the letter, where your model only has the outside of a curve and not another curve to drive the [Engrave] operation

[jfrankovich]

This is just a quick thing I put together to illustrate the problems I'm having with the engraving tool.

[jfrankovich]

I'm not sure I understand what you're saying (sorry) except that I am confused, which is 100% right.

In the video, his bit travels around the outer edge of the lettering and broken circle, which retains the original dimensions of the letters/circle while still engraving it. whereas when I do it (as far as I can tell set up the same way), the circle has been cut into, and now my circle's dimensions are less (by the cut width)

i don't think I'm explaining my issue correctly

[hyperbolicindustries]

If you want to travel around the outer edge, that is only 1 curve to control that. That is a [2D Contour] or a [Trace] toolpath. That should NOT be an engrave toolpath. Engrave is only for if you have 2 control curves AND want the tool to lift up to maintain sharp corners. Engrave operates by seeing how deep the tool can fit while still touching 2 lines. 2 lines very close together will generate a very shallow toolpath, 2 widely spaced lines will generate a very deep toolpath. That is why the N looks kind of weird, because the width is not consistent sot that the tool cuts deepen in some parts and not others.  

Its cutting to the inner edge (of the outer circle) because its is cutting between the drive 2 circles you have chosen. 

[jfrankovich]

---

@hyperbolicindustries wrote:

That should NOT be an engrave toolpath. Engrave is only for if you have 2 control curves AND want the tool to lift up to maintain sharp corners.

That's exactly what I want, but along the outside edge of my selection. For example, in my model with the N on it, I like the engraver to travel along the outside path AND raise sharp corners with the N but along the outside. The video I posted showed the guy doing precisely that. I'm wondering how to recreate that or how he did it that allowed him to do that.
I'm unsure what you mean by "two control curves," as the engraving tool works on single lines. 
I can recreate the line I want by simply figuring out the bit width and making an oversized object. But that means if I want a circle that's 5 inches wide and my bit will cut .5 inches from it, I have to set the circle to 5.5 inches to get the cut and circle size I want. that would work I suppose but would also be a pain to do on some projects. may also interfere with other subsequent cuts.

like I said, the video I posted showed exactly what I want to happen, and I set it up the same way, but I can't seem to make it work the same way

[jfrankovich]

after more testing the "just make oversized object larger than what you want to cut" sort of works except that it requires (for reasons I do not know) selecting the bottom outline of the model, not the top as well as the new sketch.

again the video i posted doesn't show those happening

[hyperbolicindustries]

In the example video he is not cutting to the outside of a continuous circle. He is cutting to the inside of a circle. The tool will try to fit inside that circle and avoid the other curves including the broken circle /arc segments and the letter outline itself. You are trying to do something different than what is in the video. Experiment with either [2D Contour] or [Trace].

What I mean about 2 curves for [Engrave] is that if you have 2 closely spaced lines/curves then the tool can only cut shallow while staying in between them. If you have 2 widely spaced lines/curves then the tool can cut much deeper. If it starts narrow then gets wider then the tool will start shallow and get deeper as the toolpath progresses. [Engrave] is a special use toolpath with more conditions needed that something simpler like [Trace] where you are just telling the tool, follow this line/curve at a constant depth.

[jfrankovich]

but I don't want to cut between the lines I want to cut outside the lines/contours tracing the circle, the N the whole thing. I could do this with trace/contour however it would not give the nice sharp corners the engrave tool does.

 this is it engraved selecting only the highlighted area as the engraving path the grey is the actual model and shows the bit is actually traveling into the intended model (and therefore cutting down its dimensions) when it cuts inside rather than around it.

 this is the same part with another N that's offset from the N I'm using in the model. the highlighted section is where the actual model is. you'll notice it keeps the sharp corners where the lines meet AND the original dimensions I wanted the N to be at before the cut.

 

The highlighted area is the N in the dimensions I want, the black outline is the offset 

 a close-up of what I want the corner to do and have done by making an offset. the highlighted area is the inside of the N's dimensions

 a still from the video showing his relief carving without needing to make an offset. you'll notice the dimensions of his model stay the same while still carving out the material around the N and T rather than inside of those dimensions.

all I want is to be able to use the engraving tool while maintaining the models specified dimensions AND getting those nice corners. to do this it just needs to calculate on the outside of the selected contours rather than the inside edge

[djlunty · Accepted solution]

@jfrankovich 

To get what you want with the engrave tool path you have to select the outside edge of the stock.  This provides the correct driving curves as discussed by @hyperbolicindustries .  The engrave tool path now knows what lines you want it to engrave between to  get the raised letter and circle that you want.  I have added  a pocket tool path with a 0.25  radial offset (calculated by this formula (tan 90/2)*0.25)   to clean up what the engrave tool path does not cut. This tool path does not get into all the corners as the bit is too big.  You could create additional pocket tool paths using REST machining with smaller bits to get into the corners.  Or you could create a fake square endmill with a very smalll diameter and use the engrave bit to get into the corners - still using REST machining.  This is the method used in the video that you referenced.  Model attached.

Your file had a 60 degree V-Bit but I changed it to a 90 degree V-Bit as that is what you said you were using . 

Looks like your letter N runs into the circle - may have to make the circle bigger to get a cleaner look or maybe it works with the 60 degree v-bit.   You could run the pocket tool path first, do the V-Bit tool path then another pocket tool path with smaller bits. 

Hope this helps.  

Attached are the file and two screenshots - one shows a cross section of the machined stock.  The other shows the remnants that need to be cleaned up with a smaller bit.

Doug