Another "inlay won't quite fit" thread - engraving bit

This forum is for general discussion regarding VCarve Pro
User avatar
JoeBlow
Vectric Craftsman
Posts: 135
Joined: Wed Nov 21, 2018 11:19 am
Model of CNC Machine: AxiomAR6Pro

Re: Another "inlay won't quite fit" thread - engraving bit

Post by JoeBlow »

I couldn't seem to grasp the "why" of using a TBN bit. The "how" I am confident can be figured out. But why?

Adze points in the right direction. In Stephan's conversation with Juan in his comments he clearly gives 2 reasons why he likes the TBN bits....

1. he can get bits with a much smaller angle than a v bit , and
2. they are stronger than a v bit.

The "how" part would take some fiddling around with settings and test samples to achieve good fitment.
Patrick

The hurrier I go, the behinder I get

aarvidsson
Posts: 30
Joined: Fri Mar 26, 2021 10:16 am
Model of CNC Machine: Shapeoko 3

Re: Another "inlay won't quite fit" thread - engraving bit

Post by aarvidsson »

Yep, that's my take on it. What confuses me to no end is while Stephan seems(?) to be using the established math (starting depth = how deep into the pocket the inlay goes, flat depth = the amount of plug sticking out) with a TBN, I can't replicate the results. With 30 degree bits I get just about the exact results I ought to get according to math, with engraving bits or TBNs, I seem to be better off creating a table of start depth / flat depth and use that. Since everything works perfectly with a 30 degree bit and so completely off with a TBN / engraving bit, I'm hesitant to attribute this behavior to inaccuracies in my machine. Trying to get hold of him to confirm.

User avatar
Adrian
Vectric Archimage
Posts: 14540
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Another "inlay won't quite fit" thread - engraving bit

Post by Adrian »

I did mention this before but I think you missed it or didn't understand what I'm getting at. I'm sure your issue is to do with the way you've broken the male part into a clearance toolpath and a final toolpath leading to the male inlay being different sizes depending on the angle of the bit used.

I've attached two pictures to show what I mean. The red rectangle represents the first toolpath with the start depth of 0 and a flat depth of 3mm. The bit on the left is a 90 degree bit and the one on the right is a 15 degree bit. The bit of material we're interested in is the one to the left of the 90 degree bit and to the right of the 15 degree bit.
Clearance toolpath.jpg
Note that the edge of the bit rides along the edge of the red vector at the surface.

Now this next picture represents a start depth of 3mm with a cut depth of 1mm. The way the software works is to "project" the vector down to the start depth so the edge of the tool is now riding along the top of the blue vector not the edge of the red vector on the surface.
Final toolpath.jpg
If the bit was an endmill that would mean the cut wouldn't change at all but with an angled bit it does as you can see from the diagram. The 90 degree bit is cutting 2mm past the edge of the vector essentially making the male plug much smaller. The 15 degree bit is cutting 0.2mm past the edge of the vector instead.
Attachments
vinlay.crv
(49.5 KiB) Downloaded 70 times

aarvidsson
Posts: 30
Joined: Fri Mar 26, 2021 10:16 am
Model of CNC Machine: Shapeoko 3

Re: Another "inlay won't quite fit" thread - engraving bit

Post by aarvidsson »

Yes - and no 😁

The CRV file I attached is a great example of how NOT to do the clearance toolpath as I completely botched the relationship between starting depth and flat depth. Stephan Forseilles shows how to do it the right way; for a 7/2 plug, he does 1.5/2 and 4.5/2 as intermediary toolpaths, and that should work.

The trouble is, even if going straight for a 4/2 plug (to sit 4mm into a 5mm pocket) or a 2/2 (to sit 2mm into a 3mm pocket), the results are the same - the plug barely clears the pocket edge and go down maaaybe two tenths of a millimeter. At the moment I'm looking at 6/2 = 3.5mm going into the pocket, 7/2 = 4mm into the pocket and 8/2 going 4.5mm into the pocket. I'm fine with trying things and creating a table that gives me consistent results, but it galls me that I can't figure out WHY I'm getting the results I am.

User avatar
Adrian
Vectric Archimage
Posts: 14540
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Another "inlay won't quite fit" thread - engraving bit

Post by Adrian »

The closer the bit is to straight the less tolerance you will get on the fit. A plug and pocket cut with a straight bit would never fit as they are exactly the same size. So basically the more acute the bit the more accurate the cut needs to be which is probably why you're getting it to fit with 30 degree bits and not with 15 degree.

I must admit I don't this type of inlay (I use the built-in inlay toolpaths) so I might be talking absolute rubbish but that is certainly what it seems like to me.

The problem with working out things mathematically is that they assume everything else is equal and, as others have pointed out, machines flex and move.

aarvidsson
Posts: 30
Joined: Fri Mar 26, 2021 10:16 am
Model of CNC Machine: Shapeoko 3

Re: Another "inlay won't quite fit" thread - engraving bit

Post by aarvidsson »

No, I think you're definitely on the money - not having any engineering background, I'm confused though; wouldn't flex show up more randomly - i.e make some parts of an inlay go deeper than others?

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Another "inlay won't quite fit" thread - engraving bit

Post by martin54 »

I must admit I don't this type of inlay (I use the built-in inlay toolpaths) so I might be talking absolute rubbish but that is certainly what it seems like to me.

I don't think your talking complete rubbish Adrian :lol: :lol: I don't do this sort of inlay either but that is what I have said in my last couple of posts, you just said it better llol

As for bit deflection & flex there are so many different factors to consider, actual machine construction is just a part of it, other factors are your z length, size & amount of stick out of bit, runout on spindle, type of material & speed, feed, DOC setting s & direction of cut to name just some of them :lol:

Flex & bit deflection can be difficult to see & measure if it's excessive then yes you may see it with the naked eye but if it is a few thousands of an inch then you probably won't & on an angled surface can be difficult to measure without special equipment.
With wood it will vary depending on the wood type & how you are cutting, climb v conventional & if you are cutting with the grain, across the grain at 90 degrees or some angle in between the two. It may cause one part to sink lower & give you a visual indication but it may not if it's only a tiny amount especially in wood or some other material with a little bit of give.

Now having said that I am not saying this is 100% your problem, just that it is possible & something you can cross off the list now with a bit of experimenting. Make a list of all the possible causes of a problem & then eliminate them all one at a time :lol: :lol:

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Another "inlay won't quite fit" thread - engraving bit

Post by martin54 »

Just a quick thought, something else worth checking wich will have a bigger impact at steeper angles is the tram of your spindle. Have you trammed the spindle on your machine?

aarvidsson
Posts: 30
Joined: Fri Mar 26, 2021 10:16 am
Model of CNC Machine: Shapeoko 3

Re: Another "inlay won't quite fit" thread - engraving bit

Post by aarvidsson »

Really great points!

I'll be toying with really shallow and easy cuts to see if anything changes. My spindle is trammed, and the runout is surprisingly good (0.02mm).

aarvidsson
Posts: 30
Joined: Fri Mar 26, 2021 10:16 am
Model of CNC Machine: Shapeoko 3

Re: Another "inlay won't quite fit" thread - engraving bit

Post by aarvidsson »

Stephan Forseilles got back to me, and it turns out that the classic Zank math does NOT work below 20-25 degrees or so for him either. His findings are in line with mine, so apparently I'm neither doing something completely wrong, nor is my machine horribly off. I'll be looking at the deflection ideas as well, but for now I'll settle for the table I've made up.

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Another "inlay won't quite fit" thread - engraving bit

Post by adze_cnc »

aarvidsson wrote:
Tue May 25, 2021 8:51 pm
it turns out that the classic Zank math does NOT work below 20-25 degrees or so for him either.
I'm not sure I like this as an explanation. Why would 30 degrees work 20-25 maybe work and less than 20 degrees not work?

My thought is in specifying the cutter (see image). The blue is a 10 deg tapered ball bit with a .25mm dia end. If tell VCarve that it is an engraving bit with a .25mm flat then VCarve will think the bit is shaped like the red line. The difference isn't much but it is an error.

You really do need to project the blue sides and measure that flat as in the link I provided earlier.
bit comparison.PNG

User avatar
Adrian
Vectric Archimage
Posts: 14540
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Another "inlay won't quite fit" thread - engraving bit

Post by Adrian »

adze_cnc wrote:
Wed May 26, 2021 2:53 am

I'm not sure I like this as an explanation. Why would 30 degrees work 20-25 maybe work and less than 20 degrees not work?
I think it's to do with my post a couple above. The method relies on the overcutting caused by using the start depth as far as I can see so the closer the bit is to a straight bit then the less effect that overcutting has. So start depth values that work with a 45 degree bit will give too tight a fit with a 10 degree bit for example.

abomb1977
Posts: 2
Joined: Sat Apr 16, 2022 7:52 pm
Model of CNC Machine: Onefinity

Re: Another "inlay won't quite fit" thread - engraving bit

Post by abomb1977 »

As a CNC Programmer by trade, I can verify that walls and chamfers are affected drastically by overly acute or obtuse angles. Any slight variations in angle or tip geometry (flats, radii, etc) will have an effect.

Keep in mind Vcarve is projecting a toolpath according to perfect conditions. As a programmer I'm constantly having to explain this to the setup guys on the floor. The math of the CAM is set to perfect by the programming. All other variables are out of our hands, but can be tracked and nailed down.

Also, I've read about people trying to check the angle of their engravers. That's nearly impossible without an optical comparator. Keep in mind that only one side does the cutting. The other side is relieved.

I myself tried jumping straight from 60 & 30 degree bits to these eye candy 15 degree ones unsuccessfully and finally had to sit down and figure out my bits. Not saying that it's all perfect, but I have found something I like so far.

I think the only way to do it, is through a controlled inlay test. Run male and female squares or shapes set to even integers to check machine accuracy. Program a male and female. I set all to 1" wide.

I set my female to 0.200, and played with depths for my male. In my case, my tools had flats, so my inlays were loose. I lessened the SD until I saw the results I wanted. Keep in mind, the SD controls the Plug engagement depth. Also, I kept adding to the FD to make sure my total depth was enough so that the base or pedestal wouldn't bottom out. I kept total depth to 0.250 for all males. Started at 0.125 SD & FD.

I hope this helps. Cheers!
Anthony

skiltrade
Posts: 36
Joined: Thu Sep 19, 2019 1:26 am
Model of CNC Machine: built
Location: Mount Prospect, IL.

Re: Another "inlay won't quite fit" thread - engraving bit

Post by skiltrade »

Howdy All,

I use this formula all the time and have no issue, it has to do with your start depth with the plug.

everything will work out weather you use a "V" cutter or a Tapper cutter (I use .025mm 7.5%-degree tapered end mill)
Attachments
20210401_195628.jpg
20201029_122303.jpg

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Another "inlay won't quite fit" thread - engraving bit

Post by adze_cnc »

Time to be a bit Socratic: in the first image if you changed the flat depth to 0.13 from 0.11 must you change any of the values in the second image? If your answer is yes then which one(s) and why?

Post Reply