CNC router - 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 (Stock to leave). 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". 

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...

Thanks in advance for any help y'all can provide!

David

[johnswetz1982]

Generally whenever someone post this it is their machine. My guess would be that your machine is losing steps as it cuts. When you just jog it the 48" it is under no cutting load which may be why you get your result. If you perform the same but actually cutting with your usual formula and at 75ipm do you get the same result or mis-sized?

[difalkner]

No, it's not losing steps.  I used the MDI window to move the 48" and 25.75" with a command of G01 F250 Y48.0, so it wasn't a manual jog.  Also, I cut the inserts twice with grain running 90° different on the second cut to rule out grain influence on the cuts.  Each piece came out perfectly cut, except for being slightly undersize, so no lost steps or it would have shown on these pieces.  In the 2+ years since I built the machine it has not lost steps, fwiw.

David

[seth.madore]

Post the file and the code that you are using, please. You might need to put them in a .zip folder and attach that here

[difalkner]

File attached, Seth.  I wonder if it will make a difference to use 3d contour and pocket...?  I used 2D to create these.  Oh, and it happens with any bit I use, pockets are always smaller than they should be.

David

[jahnj0584]

I didn't even have to check the files, but I know this is going to be a backlash issue in the machine itself. Throw a dial on your Z axis and watch as it doesn't move when you change direction.

[daniel_lyall]

Have you done a service on the machine this is always my first step?

The file looks ok but can you set your WCS in the setup.

[difalkner]

How much are you looking for?  I don't think backlash is the issue.  I just did what you said and backlash is between 0.0015" and 0.002".  I have a Harbor Freight magnetic base that's just so-so at best but a good dial indicator and I did it a dozen times.  I got 0.0025" one time but all the other times were less so maybe that's the mediocre base.

David

[difalkner]

Hi Daniel - yes, I service the machine regularly. 

The WCS is in the setups, at least as I use it, that is.  The pockets are zeroed from the top of the piece (zt in my nomenclature) and the inlay pieces are zeroed off the spoilboard (zs).  X and Y are in the direction I need them for my machine.  Am I missing something on the way WCS is set?

David

[daniel_lyall]

All the setups are like this.

What do you have the look ahead set to in mach3 or 4 I can not rember what one you have it should be around 200.

If the setps are good and everything is nices, clean and tight, look to make sure no offsets have been applyed putting G40 and G49 into the mdi and hitting enter should clear any offsets.

If all above is good do some testing in a diffrent material realy soft stuff and if the error is still there double check the tools size is correct.

I know you know this stuff already and more than likely have already done it.

[difalkner]

The 'Look Ahead Lines' default is 20, Daniel, and I left it there.  So it's been running fine for 2 1/2 years like that.  That should probably be increased but I don't think that's the issue here.

There are no offsets applied.  I don't have any soft material - mostly Walnut, Maple, and exotics.

What's wrong with the setup as I have it?  That's how I do most of what I cut, so am I doing something wrong or that could be better, Daniel? 

Thanks!

David

[difalkner · Accepted solution]

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 for backlash -

Measurements in Fusion 360 for random double curve I drew for test -

Actual measurement -

All pieces fit with no problem -

Thanks to all for your help and suggestions!  These are just test files but I certainly don't mind sharing them if you want to dive into the settings.
David

[daniel_lyall]

Good stuff

[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