CNC - calibration issues for inlays

[difalkner]

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!!!

David

[wtnhighlander]

David, could the router bit diameter be off spec? Doesn't explain your initial error when calibrating at smaller dimensions.

My best guess is that there is a small error in the gear reduction ratio of the drivetrain. I would suggest calibrating to the CENTER of the machine's range. That should at least minimize errors near the center. They will still accumulate as you travel outward, but only half as much in a given direction. 

Then I would take the caliper to the driveline parts, and see if anything is out of spec. Very small errors add up over longer distances.

[difalkner]

Yes, the bit is out of spec.  It's a 1/8" bit that measures 0.123" (last paragraph).  In the tool library I changed the spec to be 0.123" so I don't think that's the problem.  I would love for it to be something simple that I overlooked, though!

David

[Chestnut]

Fiber compression? Could the bit be compressing the fibers slightly while cutting? Are you having the CNC cut in a climb cut orientation?

I've been doing a lot of template routing lately. I'll do a first final pass pressing hard against the guide bearing. The surface doesn't look the cleanest. So i take a 2nd pass pressing hard against the bearing and every time the bit cuts more. The only thing i can think of that is happening is that the router bit is slightly compressing the wood fibers and the spring back after the bit passes.

Do you have a hard material that isn't wood that you could try this on like a hard plastic or something?

[Mark J]

I, too, was thinking the bit was smaller than spec, but then the inlay pieces would be cut oversize, not undersize.  Testing on plastic would eliminate the grain issues.  The gear comments are a good thought, too.

I'm a little suspicious of the tape measures.  You're dead on when you measure 48" with the tapes, but the tapes themselves are not necessarily accurate and in any case are not precise enough to measure into the hundredths of an inch range you need.   On the other hand I don't know of a precision instrument that will measure precisely in the 48" range.

Also you mentioned that when you use calipers to calibrate in the 6 inch range, the 48" calibration was off.  That sounds like something internal like wtnhighlander was thinking.

[difalkner]

Chestnut - I get this result with Walnut and Maple, my two primary targets for the type inlay I'll be working on soon (and have done before).  The first pass is in climb cut and leaves 0.005" on the sidewall.  The second pass is in conventional cut and removes the 0.005".  I have even run the toolpath again to see if anything else comes off the sidewall and it's a clean, no cut pass.  So to me that rules out deflection, fiber compression, machine flex (it's a stout machine so probably not much flex going on with a tiny bit), backlash, etc.  I do have some acrylic and have cut pieces out of that and they exhibit the same results - pockets are smaller than specified.

It just seems odd that I can cut Longworth chucks and other items to specific sizes - from a couple of inches to almost as large as can fit on the spoilboard and they measure precisely what I have specified.  But if I cut a pocket it's always undersized.  Inlay pieces are slightly smaller but they're closer than the pockets.

Maybe it's something I have wrong in my setup or what I have done in F360 and I hope it's something simple that I have overlooked but I just don't get it... ugh! LOL!

David

[Mick S]

David, There may be more than one issue causing the problem. First, are you measuring the diameter of the tool or the actual width of the cut it's making? They're usually not the same.

Second, if I remember correctly, you're using Fusion 360. I don't use F360 but in other CAD/CAM programs I use there's always an allowance offset for both the male and female toolpaths making up an inlay. In my classes I often see students setting the allowance value for the gap wrong by reversing the neg/pos value from what they think they're doing. That is, if they want the pocket slightly larger they set the value so that it actually leaves a smaller pocket. The reverse for the male inlay.

[difalkner]

5 minutes ago, Mark J said:

I, too, was thinking the bit was smaller than spec, but then the inlay pieces would be cut oversize, not undersize.  Testing on plastic would eliminate the grain issues.  The gear comments are a good thought, too.

I'm a little suspicious of the tape measures.  You're dead on when you measure 48" with the tapes, but the tapes themselves are not necessarily accurate and in any case are not precise enough to measure into the hundredths of an inch range you need.   On the other hand I don't know of a precision instrument that will measure precisely in the 48" range.

Also you mentioned that when you use calipers to calibrate in the 6 inch range, the 48" calibration was off.  That sounds like something internal like wtnhighlander was thinking.

I was suspicious of the tape measures, as well Mark, so that's why I used three different units made by three different companies.  One is 30', one is 25', and one is 16' - they all measured identically.  I also checked by using 10" for zero, 6" for zero, etc. just to make sure I was getting the same measurements.

I think the reason the 48" calibration was off when I used dial calipers to get the small calibration correct is that I have the reverse situation; as Mr. McCormick said, "Very small errors add up over longer distances."  When I calibrated to small pockets, which are now up to 0.015" off, then moved out to 48" then that explains why that distance is so far off.

Here's something I just did last week that shows tiny engraving on Walnut.  I ran this three times, lowering Z each time by a couple of thousandths until I got the look and depth I wanted.  If the machine had excessive play or backlash I don't think this would be so precise.

David

[difalkner]

10 minutes ago, Mick S said:

David, There may be more than one issue causing the problem. First, are you measuring the diameter of the tool or the actual width of the cut it's making? They're usually not the same.

Second, if I remember correctly, you're using Fusion 360. I don't use F360 but in other CAD/CAM programs I use there's always an allowance offset for both the male and female toolpaths making up an inlay. In my classes I often see students setting the allowance value for the gap wrong by reversing the neg/pos value from what they think they're doing. That is, if they want the pocket slightly larger they set the value so that it actually leaves a smaller pocket. The reverse for the male inlay.

I measured the tool, Mick.  I can cut a slot with the bit and it's a pretty tight fit so if the tool measures 0.123" I can't see the slot being much greater than that.

I'm not aware of any settings in F360 for male/female toolpaths for inlay work.  Typically what I do is draw the pocket to the desired shape and then create a copy for my inlay.  I then use Offset to replicate the pocket shape 0.006" smaller and that piece becomes the inlay (male) piece.  I cut those first and then do the pockets and usually have to creep up on the fit.  Using 'Stock to Leave' makes this pretty easy but it just seems like I shouldn't have to do that.  A clearance of 0.006" is sufficient for glue and should produce a nice fit if everything cut as specified.

David

[difalkner]

Let's see if I can explain what I just tested - Just a few minutes ago I cut two slots 1/8" deep 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!

David

[Woodenskye]

David, I am going to be of no help, probably why I will never have a CNC, but for the commissions you are doing, is it better to cut the pockets and then measure and write the F360 paths before actually cutting the inlay. 

[Mick S]

David, If it would help I could send you a similar file set up in Aspire with the output file to test. I would need to know what post processor you would need me to use for the output file.

[difalkner]

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 help and suggestions!  These are just test files but I certainly don't mind sharing them if anyone wants to dive into the settings.

David

[Mick S]

Glad you got it figured out!

[wtnhighlander]

Preserverance paid off! 

[difalkner]

Maybe all this will help someone else at some point.  When I do some more elaborate inlays I'll post how they come out.

David

[Chestnut]

Awesome I'm glad you figured it out.

I find myself wanting a CNC more and more for the inlay capabilities as well as the engraving capabilities. I just wish you could use a CNC with out needing to use a computer.

[wtnhighlander]

So, just "NC"?

[Mick S]

Looks like Marc just took delivery on one.

[difalkner]

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

 

[difalkner]

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.

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

[wtnhighlander]

Very clean, David. Nice job. I'm afraid I would go bonkers trying to remember all those numbers!