V-Carve Inlay Anyone?

[rlrhett]

Does anyone out there know how you would use F360 to create v-carve inlays?  For those who don't know, v-carve inlays take a positive relief and a negative relief cut with a v bit in contrasting materials.  The two are mated and one is cut or sanded away to reveal an inlay with perfectly sharp inside and outside corners.

This is a really great technique for decorative work because you don't need absolutely tiny bits to avoid rounded corners.

The Vectric software has built in scripts, but I assume it isn't too difficult to recreate the steps manually.  I'm more the artist than the computer guy so I'm having trouble thinking it through.  Logically it doesn't seem too complicated.  There are only a few things to keep in mind.  For eg. the positive shouldn't bottom out when mated so that you can be assured of a good fit.  Is there an evangelist out there who knows how this is done?  Here is there Youtube video on how Vectric has done it:

[michallach81]

Now @HughesTooling

Mark, I've used offset in pocket not without a reason. Main reason was to point how important in that Inlay method, is to know what chamfer mill we using (angle and diamater), and knowing what are  the consequences of that. If @rlrhett would trail trough finding right offset for right depth he would know how the male part was build.

In your first example after all changes you've made the male part useless. Because in engrave tool we can't choose any radial offset (both in Fusion and in Vcrave) we have to play with depth. Since we are using a tapperd tool, we can have radial offset achived by changing the depth... because you've overlooked that, this is how our parts differs one from another:

Just watch your screencast (post #11), and you will see how at the end your male part is look like, and how dose it looks in a vid from first post.

Because I was afraid that @rlrhett would fall in the same trouble as you, I was wishing that trailing through setting pocket, would help him understand the principles.

Similar choise I've made when I've picked outline to revers area for pocket. Only reason was to make it similar to Vcrave workflow, not to bring more confiusion. I could also do all cam without a single body. Sketch would be enough, but it tooks more time, and it's less obvious. As I've mentioned I was making that screencast at work, where I don't have microphone, so video had to be sort and clear, because I wasn't able to add any comments.

Answer about "prismatic overcut" is trivial, but I will post that in next replay. Hold your breath.

[michallach81]

Hi @rlrhett

In your last video "prismatic overcut" is intended gap between male and female part:

To know how much we have to raise or lower chamfer mill we need to count lenght of diagonal, these are the simplest methods:

Program in the video do that for you... but whole process is unnecessary

, when the easiest way is to raise ready male part above female part... it will mean the same. There a no special reasons for cutting with offset, when it's enough to place distance between parts.

Off topic... don't hold your breath for so long, I had problems with power supply, here at work... I've just find laptop and used my smartphone as a hotspot.

[michallach81]

I have to correct myself, in that "swirl man" video when they say "prismatic overcut" they mean gap between parts but not in cavity, which is exactly opposite of what I've guessed it supposed to be, my bad. Now it's even more trivial, cause setting from my screencast (post #7) will give you 0.1inch gap, and parts in cavity will be tight.

[rlrhett]

I hope you don't mind, Michal, but could you walk through some of the decisions you made to create the part.

1. In the fist setup, you chose only the main body to do a flat pocket cut.  How did you know that only that one section would need the flat pocket?

2. In radial Stock to Leave you chose .2, which matches the depth of cut.  Is this because you had a 90deg v-bit?  What math would you do if you had a 60deg or 40deg to know how much offset?

3. On the male part, you choose to mill the flat parts to the same .2 depth, but with half the offset of the female part.  Radial offset is .1".  I am assuming that is to account for the problem of the parts not bottoming out mentioned in my earlier post, but how did you arrive at this value?

4. On the v-bit engrave you set the bottom to be .1" but also offset the top by .1".  Again, I don't understand these values.  What does the top offset do?  How is this different than just setting the bottom to .2"?

Thank you so much for your help.

[HughesTooling]

Hi Michal

Thanks for explaining where I went wrong, at least @rlrhett got a lesson in how not to do it.

If I've understood correctly setup1 (female side) works OK how I did it as that side is just a standard engrave. Using the taper pocket option makes it a bit easier if you use a different angle cutter.

For setup2 (male side) you need to machine under size, I understand how you've done that but I think I have a slightly easier way. If you move body2 up by half the depth of cut for the female side, in this case 0.1" you can still use taper pocket and engrave and get the same result you did. You just set the Top Height to Stock Top and the Bottom Height to Selected - 0.1".

For the Engrave op you set Top to Selected contours and Bottom to Selected contours -0.1"

I've done a screencast, messed up a bit on the 2d pocket, I clicked rest machining by mistake and it took me a while to figure out what was wrong.

I've attached a file with 2 setups for 45° and for a 60° cutter, if I've got it right all you need do is change the angle in the 2d pocket multiple stepdown to match your chamfer cutter.

Mark

[daniel_lyall]

V carve inlay is a hard one unless the program is built for it.

[michallach81]

I would say, unless you konow how it works, or even I would say that it's simple and there are just few rules to follow.

[daniel_lyall]

I give you that one there are rules to it

[michallach81 · Accepted solution]

Sure:

 1. I've used same sizes and settings like in this "bird" video, and I saw that only that biggest outline would reqiure pocket. Of course in any other exapmle you would have to pick all outlines.

 2. tg α = a/b, where a and b are witdh and depth, α is an angle, value for tg 30º= √3/3 ; tg 45º= 1 ; tg 60º= √3... but don't bother to count that, there's a simpler way to do it. I sell you that tip at the end. 

 3 and 4. Not exactly... to be honest I just used values form first vid, assuming that they should works. Nevertheless there are prinicples to follow.

Whole trick is about know how Engrave tool is working. Take a look at image below:

fig. 1

Blue dots represents our outline in a section view. Left on side we can see ordinary example where distance between opposite sides of outline is smaller then chamfer mill diamater. Right on side is an example where that distance is larger then diamater. Engrave tool would still be able calculate that path, because it always calculate (even left on side one) "imaginary" cone that our taperd tool is creating (green dashed line). This drawing (fig.1) is just section view, to understand how that cone is used to calculate path, you need to see it from above:

 

fig. 2

As you saw I draw two circles and apply tangent constrant, the Engrave path always match circles center points. This is how Engrave works, abstract/"infinite" cone fills in outline (my english and math vocabulary is too modest to make it more accurate description,  I do apologize).

If so, then way we can see examples like this?

fig. 3

Principle is the same, but Engrave tool add one more setting, which is Bottom Height. That limits the depth, up till which, chamfer mill can get. Value for that is based on chamfer mill size, it lefts some room above Top Height. I'm guessing for chips to fly off:

fig. 4

We can of course overwrite that, by changing value or reference plane (by default it's Top Height):

fig. 5

Now we can get to finding how to set female and male part for inlay.

fig. 6

On a drawing above cutting female part is easy, you picking outlines, setting depth (Bottom Height) and that's it (Note that depth must be equale or less than value that Engrave tool made default, if you'll find yourself in need to get deeper you should take bigger chamfer mill).

Problem occurs in making male part. With the same settings as for female part, male part would be to big to fit. Only way to achive proper part is to cut deeper:

fig. 7

For this to happend, we must first lower both depths (Bottom Height and Top Height):

 

fig. 8

This will force Engrave to be calculeted from new lowered plane (fig. 9, below):

fig. 9

If we would lower only the Bottom Height, we would calculate from same plane but to a different depth (fig. 10):

fig. 10

Last thing is to set Pocket. On female part your setting Bottom Height with same value as for Engrave, and the offset is a =  tg α * b, where α is half of chamfer mill angle, and b is the depth... don't like math? Watch:

fig. 11

That was easy, isn't it? Male part? Now it's your time to find.

My promised tip is to use section view to know exact values, draw your problem in real scale and you will find depths and offsets.

To sum up, all these may look complex but it's simple indeed. I'm sure we can find more streamed workflow with clear steps and formulas to apply, but currently I don't have time to find right tools & tricks.

[rlrhett]

Brilliant! Thank you.

PS. What is your native language? I did notice some awkward phrasing, but assumed it was just engineer speak. I am very impressed with your explanation, and doubly so considering it isn't your native tongue.

[michallach81]

I'm a Polish. I do feel confident with my english, and do think I have rich vocabulary, but I do struggle with grammar, especially with reported speech.

What's your nationality?

[daniel_lyall]

@michallach81 ask the mods to take your post out 29 and move it to tips and tutorials it's good.

[balunist]

Mark,

Thank you!!  This is exactly what I needed.  I love the use of Mirror in it's creation.   

[Anonymous]

Sorry to bump this thread, but I've been trying to do some inlay work with a 60 Degree bit using all the info in this thread but it doesn't seem to be correct.

The suggestion to use wall taper angle, doesn't that result in a male part that is oversized? Really having difficulty finding the engraving offsets for the male feature.

I am machining the pocket to -.2. and setting the engraving as below:

Top Height Offset: -.17125

Bottom Height Offest from Top Height: -.02875

Any suggestions on these?

[rlrhett]

All I can say is that if you follow the excellent post marked as the answer you will get matching parts.  Check your math.  I have used that method with a 60deg bit successfully dozens of times now.

One little bit of unsolicited advice:  I would not use a 60deg bit, at least not on wood.  I did several parts that way thinking I would get a deeper inlay and more material in the narrow parts.  It's true, I did.  But the taller and thinner male/positive part was also a lot more prone to blowing out when actually milled.  I tried sharp bits, very slow speed, very fast spindle.  It was rare that I got a part that didn't have problems in narrow parts.  Since I did a number of nautical motifs with ropes and other thin and long inlay, this was a constant issue.  Finally I had a hunch that the problem was the 60deg bit and switched back to a 45deg bit.  Problem solved.

The added bonus is that if you are using a 45deg bit the math is much easier and you are less likely to make a mistake.

[Anonymous]

rlrhett,

I was able to work through some of the math, but still a bit lost. My inclination was to try a 45 degree bit next for the very reason of simplifying it.

Thanks for the quick tip.

-Ross

[Anonymous]

I've been trying to figure this out for a couple hours now to make the embossed part and can't figure it out. Keep in mind I've only been CNC'ing for about 6 months now, but I've done engravings before, just trying to wrap my head around making the inlay part. Thanks for any help! 

I've included a simple example file. If anyone has the time to do a screencast/youtube video of how to get the embossed part made from the example file, I would surely appreciate it!!!!! 

EDIT: I looked at the other screencast and that helped a lot, but I'm still hitting roadblocks because of my inexperience. I watched the youtube video of the guy doing it in vcarve, but I couldn't find any videos on youtube of people doing this in Fusion 360, and I'm not about to shell out $300 for something I know can be done in fusion! Something with someone talking about what they're doing would also really help. Sorry if this is too much to ask, I'm just having a lot of trouble following the screencast! 

[Anonymous]

So I've been tinkering around with it for a couple more hours. I think I got it to work properly, but I need to know if I did everything alright. I don't know if this is the proper way to do it, or if I'm missing a few steps. I know the term prismatic overcut so that you can get a proper glue-up, and don't know if the way I did it is the right way. I've included the file so if anybody has a minute to check it out, I'd appreciate it, thanks!!! 

[WhiteRoomSkis]

Bumping this to get feed back on this tutorial

So after a bunch of reading and a bunch of trial and error I came up with this brief tutorial based on this thread with a bit of my own observations and expanded explanations. Please correct anything you see wrong here. I am by no means an expert in the method. This was my first try at it. I figured if I was struggling with this others might be also.

• Fusion 360 v-carve inlay tutorial
• Create your geometry copy and mirror it, paste it next to the original you'll need them both for the male and female parts.

Female component

Set up a 2D pocket tool path 

• use an inside vector. Run this program first. This will make it easier for your V-bit to cut in the next step.
• Set your depth of cut to your desired depth. I cut this slightly deeper then the male component by .5mm-1mm to allow the male portion to fully seat within the pocket.

Set up an engraving tool path

• nothing special here, just engrave as usual with the same depth of cut as above to clear the sharp corners in your part.
• Set the top height below your stock top. You will need to lower this until your inside edge is fully chamfered. This usually works best if your top height and bottom height are the same. i.e.top and bottom height  are both -5mm. Don't worry about bogging down your bit, remember you have already cleared the center of the part with the pocket tool path.

Male Component

Set up a 2d pocket tool path

• Set this up for outside contours and also select the stock boundary to clear the un-needed stock.
• Select multiple depths. set your depth to your maximum roughing depth to your desired depth, somewhere between 1-2mm should be fine for this.
• Set up a wall taper angle which is 1/2 of what your tool angle is. For example a 45 deg wall for a 90 deg too and a 30 deg wall for a 60 deg tool etc. 
• Select radial stock to leave and add the same amount to leave as your depth of cut if using a 90 deg tool.                   Depth of cut = 5mm then also leave 5mm of radial stock.
• If you are using a different angle tool (60 or 45 deg) the amount of stock you need to add will be different.

Set up an engraving tool path

• Select your geometry as usual, Also select the stock border which will allow your tool to chamfer the outer border of your part
• set your bottom depth to the desired depth of cut for your part.

female and male parts

mated parts

[WhiteRoomSkis]

Edited process

• Fusion 360 v-carve inlay tutorial
• Create your geometry copy and mirror it, paste it next to the original you'll need them both for the male and female parts.

Female component

Set up a 2D pocket tool path 

• use an inside vector. Run this program first. This will make it easier for your V-bit to cut in the next step.
• Set your depth of cut to your desired depth. 

Set up an engraving tool path

• nothing special here, just engrave as usual with the same depth of cut as above to clear the sharp corners in your part.
• Set the top height below your stock top. You will need to lower this until your inside edge is fully chamfered. This usually works best if your top height and bottom height are the same. i.e.top and bottom height  are both -5mm. Don't worry about bogging down your bit, remember you have already cleared the center of the part with the pocket tool path.

Male Component

Set up a 2d pocket tool path

• Set this up for outside contours and also select the stock boundary to clear the un-needed stock.
• Select multiple depths. set your depth to your maximum roughing depth to your desired depth, somewhere between 1-2mm should be fine for this.
• Set up a wall taper angle which is 1/2 of what your tool angle is. For example a 45 deg wall for a 90 deg too and a 30 deg wall for a 60 deg tool etc. 
• Select radial stock to leave and add the same amount to leave as your depth of cut if using a 90 deg tool.                   Depth of cut = 5mm then also leave 5mm of radial stock.
• If you are using a different angle tool (60 or 45 deg) the amount of stock you need to add will be different.

Set up an engraving tool path

• Select your geometry as usual, Also select the stock border which will allow your tool to chamfer the outer border of your part
• set your top height to -.2mm. this will create a slightly smaller male part and allow the part to be closely mated.
• set your bottom depth to the desired depth of cut for your part.