# CNC - calibration issues for inlay work



## difalkner (Jan 3, 2012)

This is puzzling to me... I can scribe a line on my spoilboard, move the Y axis 48" by command line, scribe a line there and it measures exactly 48". I can do the same with X and move 25.75" and the measurement appears perfect. I am using a tape measure because that's all I have for measuring that distance. However, I used 3 different tape measures by 3 different manufacturers and each one measures identically.

But, and this is a big 'but' to me, if I am cutting a pocket it ends up being undersized. Same with an inlay piece - undersize. I can compensate in the software (Fusion 360) but I shouldn't have to do that. If I cut a 1" square for an inlay piece and specify a 1.006" pocket then the inlay should fit with 0.003" clearance all the way around - it doesn't.

I understand different woods, grain is hard in some areas, soft in others, cutting with the grain, across the grain, etc., but generally a 1.006" pocket should be 1.006", not 0.993". And a square inlay piece that is programmed to be 1" should end up being 1", not 0.992". Also, it's safe to say that all I cut are hardwoods and they hold their dimensions better.

With simple shapes like squares, rectangles, circles, etc. it's easy to make them fit. But when I need to do complex shapes - music notes, arcs, a deer or car - it's very difficult to make these fit and sometimes downright impossible.

When I first calibrated the CNC after I built it I did all my calculations under 6" so that I could use my dial calipers. What I found is that I could get it spot on for a 4" square, for instance, but if I needed to cut something 48" in the Y direction or 25" in the X direction it was off by 1/8" to 3/16" and that's simply unacceptable. So I did it the other way - I made the greatest distances as accurate as I could get them figuring that the smaller dimensions would now be very close if not perfect (within tolerance for the machine, of course). 

I have a few projects coming up with multiple inlays in each, probably 20-30 inlays and they're all different shapes and sizes, so I need to get this right. Today I cut some test pieces using a bit that measures 0.123" - a downcut 2-flute spiral - and climb cutting a rough pass leaving 0.005" on the side walls. Then I followed up with a clean up pass in conventional cut to remove the final 0.005". I figured that should take out any flex issues on the bit and also compensate for different grain directions. The feed rate was 75 ipm so not very fast. I was more concerned about pieces being accurate than being cut fast.

Inlays fit but are undersized -








Measurements of pockets and inlays - 








Using 2" as zero to test Y axis calibration -








Moved 48" and this appears to be perfect - 








Using 2" as zero to test X axis calibration - 








Moved 25.75" and this appears to be perfect - 








Setup for X axis calibration - 








So how can I get these inlays and pockets to be correctly sized? This generally isn't affecting the Longworth chucks I cut so many of and it certainly doesn't affect plaques or signs. But I don't see how it can be right at the greater distances but off on the smaller distances. I also see this when I need to cut a larger hole to fit a dowel, say 1 1/4". If I specify the hole to be 1.260" to give a little clearance then what I find is the hole comes out 1.235" to 1.240". 

Help!!! :crying:

David


----------



## PhilBa (Sep 25, 2014)

Is "Stock to leave" checked? That bites a lot of people. I managed to check it once without realizing it. Scratched my head for several hours before noticing it. I think .01 is the default for inches.


----------



## difalkner (Jan 3, 2012)

No, not on the finish pass, Phil. Default setting is 0.02" and I use it all the time for various tasks. In this case I used it on the rough pass to leave 0.005" on the sidewalls and then cleaned that up on the finish pass.

David

Edit - Is this a Fusion 360 issue? When I moved the carriage 48" and 25.75" I did it by command line so Fusion 360 wasn't involved. I suppose I could replicate the 48" and 25.75" test in F360 and see if that works as it should...


----------



## PhilBa (Sep 25, 2014)

OK. I use MM and it's 1 mm default on StL. I see people saying my "20 mm pocket is 18 mm" or similar and it's always StL checked.

I've got a similar one where VCarve is .2 mm too high. I'm still learning VCarve so it's probably a bonehead newbie mistake. I lie to my machine and tell it zero is .2mm lower than it is. Not a good way to run a railroad though.


----------



## PhilBa (Sep 25, 2014)

Maybe a dumb question but have you measured the actual width of a slot cut with a single pass? That seems like a huge amount to be off but not completely impossible.


----------



## kp91 (Sep 10, 2004)

Spindle run-out or bit dimensions not exactly equal to what they are supposed to be?


----------



## TimPa (Jan 4, 2011)

i think you'll find that one factor is the cut direction. a "climb" vs "conventional" as the last cleanup pass of the pocket will have an effect of a few thousandths on my machine. one direction has the bit pulling into the wood, and the other is pushing away, give it a try...


----------



## difalkner (Jan 3, 2012)

PhilBa said:


> Maybe a dumb question but have you measured the actual width of a slot cut with a single pass? That seems like a huge amount to be off but not completely impossible.


Yes, and it's exactly the size of the bit. Or at least, it's as close as I'm able to measure.



kp91 said:


> Spindle run-out or bit dimensions not exactly equal to what they are supposed to be?


I don't think there's any spindle run-out. I'm able to engrave very tiny letters with no wobble shown in the final result.










TimPa said:


> i think you'll find that one factor is the cut direction. a "climb" vs "conventional" as the last cleanup pass of the pocket will have an effect of a few thousandths on my machine. one direction has the bit pulling into the wood, and the other is pushing away, give it a try...


Yes sir, that's why I do the rough cut in climb and the finish cut in conventional. And the finish pass is only taking 0.005" so it's a very light cut.

One thing I haven't tried is to change the profile of the cut. I cut these using 2D pocket and contour but I may try them using 3D pocket and contour.

David


----------



## Pro4824 (Oct 17, 2015)

Process of elimination...
You can manually move 48" (or any distance) accurately? Then the old blue tank has no issues. So it's a F360 issue. Didn't you get Carveco? If so, have you tried duplicating the issue with it?


----------



## tooler2 (Aug 11, 2012)

If you are going to be measuring in such precise dimensions I think you should buy a set of gauge blocks. A dial caliper is not the way to go as the knife edges will penetrate the wood differently every time. Likewise the diameter of the cutter is less important than the actual kerf width when calculating offsets and gauge blocks will be the best method for measuring.
Rob


----------



## difalkner (Jan 3, 2012)

Gauge blocks won't help much, Rob. These are simple shapes I used for testing but I rarely inlay squares and circles. Most of what I do is irregular shapes. The dial caliper gives me an idea of sizing, though. If anything, using the dial caliper on a pocket should give me a reading closer to spec if I am cutting into the wood (I don't really think I am, though - being very careful). On the inlay pieces I use the thicker flat portion of the caliper jaws.

This particular cutter measures 0.123" and when I cut a slot in one direction, then take the bit out to test the fit I find it to be a good fit. Not sloppy or loose and certainly not such that I have to force the bit to make it fit. And it doesn't matter which bit I use, pockets are always smaller than specified.

David


----------



## difalkner (Jan 3, 2012)

Pro4824 said:


> Process of elimination...
> You can manually move 48" (or any distance) accurately? Then the old blue tank has no issues. So it's a F360 issue. Didn't you get Carveco? If so, have you tried duplicating the issue with it?


I used the MDI window and a command of G01 F250 Y48.0 to move to the 48" mark and G01 F250 X25.75 to move to the 25.75" mark, and it went to the exact same spot several times. So I agree, ol' blue is doing its thang correctly.

I'm not sure on F360, I wonder if using 3D to create the pockets and contours would work better than the 2D I used on this...? 

Yes, I got Carveco but sadly, at this point I but the tiniest of a clue how to use it! LOL! :crying:

David


----------



## tooler2 (Aug 11, 2012)

difalkner said:


> Gauge blocks won't help much, Rob. These are simple shapes I used for testing but I rarely inlay squares and circles. Most of what I do is irregular shapes. The dial caliper gives me an idea of sizing, though. If anything, using the dial caliper on a pocket should give me a reading closer to spec if I am cutting into the wood (I don't really think I am, though - being very careful). On the inlay pieces I use the thicker flat portion of the caliper jaws.
> 
> This particular cutter measures 0.123" and when I cut a slot in one direction, then take the bit out to test the fit I find it to be a good fit. Not sloppy or loose and certainly not such that I have to force the bit to make it fit. And it doesn't matter which bit I use, pockets are always smaller than specified.
> 
> David


The gauge blocks are for calibration purposes not for regular use. As a tool and die maker I would not use a caliper to measure your bits and besides it is the width of the slot that counts and material cut probably changes width of the slot. Even milling steel on a rigid milling machine we will cheat on the tool diameter input to correct for offset. You should also calibrate your caliper at various openings using gauge blocks. Most of the time when measurements don't make sense it is a problem related to taking the measurements in the first place and very few woodworkers have studied metrology in depth.


----------



## stevenrf (Jul 30, 2010)

I think you should use a machinist micrometer to exactly measure bit diameter.


----------



## difalkner (Jan 3, 2012)

If I had one I certainly would but even with my dial calipers I doubt I'm more than 0.001" off, if that. What I'm talking about here is way more than missing bit size by one or even two thousandths.

David


----------



## difalkner (Jan 3, 2012)

tooler2 said:


> The gauge blocks are for calibration purposes not for regular use. As a tool and die maker I would not use a caliper to measure your bits and besides it is the width of the slot that counts and material cut probably changes width of the slot. Even milling steel on a rigid milling machine we will cheat on the tool diameter input to correct for offset. You should also calibrate your caliper at various openings using gauge blocks. Most of the time when measurements don't make sense it is a problem related to taking the measurements in the first place and very few woodworkers have studied metrology in depth.


I have one gauge block/bar, a 1" round one marked 1.0000" 25.40mm HSS. When I measure it with my calipers they show exactly 1", dead on the money. Close enough for what I am doing, I would say. I was a machinist for a while before getting into injection molding and working with the tool & die team on a regular basis and probably closer to engineer/machinist than I am traditional woodworker. My medium of choice just happens to be fine hardwoods and exotics. 

But I very definitely understand and agree with what you're saying and don't take it lightly. It's just that I don't think missing the bit size by 0.001", if that, is the error I am seeing. 

Let's see if I can explain what I just tested - Just a few minutes ago I cut two slots with this 0.123" bit in hard Maple, one with the grain and one across the grain. Now, I don't have a good way to measure that slot other than my dial calipers so I used a 1/8" carbide bit shank, measured it to be 0.124", and it fits in the slot with the grain with a little wiggle room as I would expect. On the slot across the grain it fits like a glove. 

At this point I used feeler gauges and set beside the shank to press both into the slot with the grain. At first I tried 0.0015" and it's loose so I tried 0.002" and it's a good fit. I tried 0.003" and I can't get the two into the slot without tapping it in with something harder than my finger and at that point I would probably be compressing wood fibers. With the 0.002" feeler gauge the slot with the grain fits like the slot across the grain. So that tells me this 0.123" diameter bit is cutting a slot about 0.126" wide with the grain and right at 0.124" across the grain and that's about what I would expect.

I don't think it's a measurement or machine issue but rather something to do with Fusion 360 and the way it's telling the CNC to cut. But I will find it, sooner or later, I will find it!! LOL! :grin:

David


----------



## tooler2 (Aug 11, 2012)

I know nothing about the software, but for others reading this I should point out that the tangent point of a 1/8 bit is not a great way of measuring a slot width in a soft material any more than a sharp caliper is. Gauge blocks are cheap now!


----------



## difalkner (Jan 3, 2012)

It's the best way I have, Rob, so today it's going to have to do. :wink:

David


----------



## difalkner (Jan 3, 2012)

Ok, found it!!! At least, my tests are now working as designed. I'll try some more complex shapes later. 

Here's what I found - I recall reading somewhere that there's a difference between 2D and 3D Contour in Fusion 360 and that 3D is more a finishing profile. But 2D works for what I have needed about 99% of the time and that's what I use. Plus, you can have tabs in 2D but not 3D. I'm not certain where I read/heard that but I couldn't find this again in a quick search so I'll look later. Backlash has been discussed amongst the folks I queried on this so I tested that, as well. It was very minor - 0.001" to 0.002".

Inlay - For the inlay piece I used 2D Contour and my standard climb cut with 0.005" Radial Stock to Leave for the rough pass followed by 2D Contour conventional cut to remove the final 0.005". The inlays, while slightly off, have not been the issue; the pockets were.

Pocket - I created a profile for 2D Pocket climb cut to clear the inlay pockets with Stock to Leave set to 0.005" Radial. I followed that with a 3D Contour conventional cut and no Stock to Leave plus selected Repeat Finishing Pass to clean up the sidewall. This makes the cutter go around the sidewall twice, so even if the 0.005" clean-up pass had any deflection the second pass around should take care of that.

The pockets now measure what I have specified in F360, or as close as I am able to measure. The important thing is that now the inlay pieces fit with no problem. I even placed my 1" round gauge bar in the 1" pocket and it fit (snug, but it fit).

1" gauge bar in pocket - 








Testing backlash - 








Fusion 360 measurement for random double curve I drew for test - 








Actual measurement - 








All pieces fit as needed, no forcing, not a sloppy fit, just right for glue - 








Thanks to all for your suggestions!
David


----------



## BalloonEngineer (Mar 27, 2009)

You will find it is much easier to get good quality inlays using the VCarve inlay technique. Can also do sharp corners. 





Skip Fusion for this and do it in Carveco.


----------



## Pro4824 (Oct 17, 2015)

Congratulations David, that's great to hear. We want pictures of the inlay projects!!


----------



## honesttjohn (Feb 17, 2015)

With Vectric they ask if you want to cut "inside" the line or "outside" the line. Don't know if your programs have this or not.


----------



## PhilBa (Sep 25, 2014)

BalloonEngineer said:


> You will find it is much easier to get good quality inlays using the VCarve inlay technique. Can also do sharp corners.
> 
> Skip Fusion for this and do it in Carveco.


I've used that technique. Also supported in F-Engrave, for a free option. It's a reasonable and fairly easy approach but has some limitations that should be considered. You need to cut the inlay off the bottom once glued in place. There's a reason why the videos out there use coasters as an example - easy to put through the band saw. Much harder to do for a larger piece like a table or desk top. I've used a flush cut saw but it takes care to get a really close cut without marring the base. If you don't, you're in for a major sanding/scraping session. I'm sure a lot of people go at it with a ROS like in the video but I'm not a fan of aggressive methods on inlays. Another problem is the need to really clean up both the inlay and base carvings for gluing. It doesn't take much to cause a gap which is why the guy in the video doesn't like Titebond III which cures dark and is more obvious. And chipping or even small tearout can be pretty obvious. And you have to be very careful to not get any chips or debris in the glue which causes gaps also. If you look closely at the coaster in the video you can see minor issues in several places. Not terrible but if you're a perfectionist it's something to consider. The other thing is it's a blind operation - you can't really see how good the fit is until you cut it open.

David's approach allows for more precision and sharp corners can be had with a little chisel work. If you use a 1/8" bit, the clean up is pretty minor. Though, his approach is a lot more work in general.


----------



## Oscar36 (Feb 23, 2019)

Always beautiful work so can't wait to see what art you make with the inlays.


----------



## difalkner (Jan 3, 2012)

honesttjohn said:


> With Vectric they ask if you want to cut "inside" the line or "outside" the line. Don't know if your programs have this or not.


Yes sir, it's not that simple, though. You just choose different profile types in most cases but we do have the option to cut inside, outside, or on the line in many profiles. Fusion 360 has like a dozen options attached to every option, nothing wizard driven or chosen for you. 

A good thing about F360 is that there are tons of different ways to skin that cat. A bad thing about F360 is that there are tons of different ways to skin that cat. :wink:

David


----------



## difalkner (Jan 3, 2012)

We've been gone all day down to Natchitoches to tour a shop and a couple of galleries as part of our Woodworking Club we started a little over a year ago. Saw some really cool shop designed and built equipment, too - old iron!

Anyway, now that we're back home I headed out to the shop to do a more complex inlay with my newly discovered technique. This is a treble clef about 7" tall and a lot going on for an inlay. I cut the treble clef and promptly broke it in one place so ignore that. I figured it would suffice for my test. I cut the pocket just like I did on the earlier simple test - 2D Pocket to clear followed by 3D Contour with two passes around the sidewall. It was snug but fit, so I did another pass on the sidewall with Stock to Leave set at -0.001" and now it fits just fine. 

Since I don't want to break it again I didn't press it into place fully but it does fit with enough room for glue.

















I'll do some others later.
David


----------



## Oscar36 (Feb 23, 2019)

David, really nice project. Thanks for sharing.

Sad I couldn't make the trip down. I was hoping to look at the rocking chairs. Beautiful design.

Oscar


----------



## HDVideo (Mar 8, 2018)

Thanks David, for creating this post and finding the problem! I just discovered this exact problem on my machine a few days ago and hadn't had time to try to figure out what was going on. I'll be in the shop today to test your theory.

Ed


----------



## HDVideo (Mar 8, 2018)

Can someone explain this:

Cuts using 2D contour with Horizontal and Vertical Lead In/Out set to .0125", the tool path is what I would expect. Ramp option is not selected.

But using 3D contour using the same Lead In/Out settings, the horizontal Lead In is much greater than specified on two of the shapes and a Helical Lead In is used on the other. The Ramp option is turned on by default in 3D contour and cannot be de-selected. 

Why are two different Lead In strategies used when 3D contour is selected? I'll post this in the F360 FB group as well to see what explanations they may offer.


----------



## difalkner (Jan 3, 2012)

Not sure, Ed. I drew something similar and got the same results. However, I rarely use Lead In or Lead Out. 

I created the 3D Contour toolpath, left Helix selected, set the ramp to 10°, and it acts very much like a 'soft' lead in.









Btw, I also rarely leave the ramp at the default 2°. Most of these defaults are for cutting metal. My ramps are usually 10° to 30° or I use Plunge.

David


----------



## HDVideo (Mar 8, 2018)

difalkner said:


> ...I rarely use Lead In or Lead Out.
> 
> David


As you, I generally turn Lead In and Lead Out off, but for this quick test didn't bother, and was confused with the result. Thanks for confirming that you see the same thing.

Ed


----------



## Traupmann (Jun 14, 2013)

*Sketchup Addict*



tooler2 said:


> If you are going to be measuring in such precise dimensions I think you should buy a set of gauge blocks. A dial caliper is not the way to go as the knife edges will penetrate the wood differently every time. Likewise the diameter of the cutter is less important than the actual kerf width when calculating offsets and gauge blocks will be the best method for measuring.
> Rob


I'm not in agreement about the calipers statement. I agree with the rest.
One should get repeatability with calipers used correctly. Never use force that will cut into the wood, measure in several places at various angles for a consistent reading. Wood is not like metal, various forces make for an uneven surface (under a microscope). Gauge blocks will force some of the narrowness to flatten -- hence, a good measurement!


----------



## difalkner (Jan 3, 2012)

Here's an update on the inlay testing using some Walnut and Maple. I had a few minutes this afternoon and cut a small circle, an arc, and a larger circle (think, portion of a Longworth chuck).

All the settings were as I specified before but ignore the first set of pockets. No matter how much you 'know' what to do if you type the wrong values the pocket won't be the correct size. :surprise:

The pockets are 0.006" larger than the inserts and fit nicely (0.003" per side). I really could make it 0.002" per side but 0.003" certainly makes it easy to get the inserts in with glue. The pockets are 0.150" deep and I cut the inserts 0.1875" thick to leave a little sticking out for sanding flush. Also, I cut the inserts upside down so I don't have to clean up the tabs and the extra 0.0375" is enough that I can lightly trim them and the inlay fits.

I glued these into place, gave a quick 5 minute French polish (2# cut, light amber color), and took some photos, so nothing elaborate but you'll get the idea. I'm pleased with the fit on these inlay pieces.

























David


----------



## Oscar36 (Feb 23, 2019)

David, very nice. That is tight!

You are "almost" inspiring me to go back and try figuring out how to do inlays on my machine correctly and then I remember how much work they are to do.


----------



## difalkner (Jan 3, 2012)

Once you get the numbers to work for you, Oscar, then it's just a matter of applying that to each shape. I may create a template in Fusion 360 to shorten/quicken the process.

David


----------



## mkoukkgou333 (Feb 21, 2020)

i also think you'll find that one factor is the cut direction.


----------



## difalkner (Jan 3, 2012)

mkoukkgou333 said:


> i also think you'll find that one factor is the cut direction.


Which is why I covered that in the very first post - climb cut first pass, conventional cut final pass.

David


----------

