Router Forums banner
1 - 20 of 37 Posts

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #1 ·
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 -
Tool Metalworking hand tool Wood Cutting tool Tool accessory

Measurements of pockets and inlays -
Calipers Metalworking hand tool Tool Ruler Tool accessory

Using 2" as zero to test Y axis calibration -
Ruler Tool Measuring instrument Calipers

Moved 48" and this appears to be perfect -
Ruler Measuring instrument Tape measure

Using 2" as zero to test X axis calibration -
Measuring instrument Tool Ruler

Moved 25.75" and this appears to be perfect -
Ruler Measuring instrument

Setup for X axis calibration -
Tool accessory Workbench Tool Machine Table

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
 

·
Registered
Joined
·
1,552 Posts
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.
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #3 · (Edited)
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...
 

·
Registered
Joined
·
1,552 Posts
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.
 

·
Registered
Joined
·
1,552 Posts
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.
 

·
Registered
Joined
·
198 Posts
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...
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #8 ·
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.

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.
Wood Wood stain Text Hardwood Plywood

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
 

·
Registered
Joined
·
413 Posts
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?
 

·
Registered
Joined
·
124 Posts
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
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #11 ·
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
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #12 ·
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
 

·
Registered
Joined
·
124 Posts
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.
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #15 ·
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
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #16 ·
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
 

·
Registered
Joined
·
124 Posts
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!
 

·
Administrator
David
Joined
·
3,976 Posts
Discussion Starter · #19 ·
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 -
Workbench Tool Tool accessory Wood Table

Testing backlash -
Gauge

Fusion 360 measurement for random double curve I drew for test -
Text Line Font Diagram Screenshot

Actual measurement -
Calipers Tool Gauge Measuring instrument

All pieces fit as needed, no forcing, not a sloppy fit, just right for glue -
Wood Font Table Plywood Wood stain

Thanks to all for your suggestions!
David
 

·
Registered
Joined
·
372 Posts
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.
 
1 - 20 of 37 Posts
Top