Page 1 of 5 12345 LastLast
Results 1 to 15 of 67

Thread: CNC - calibration issues for inlay work

  1. #1
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    652

    CNC - calibration issues for inlay work

    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 -
    001 - Inlays fit but are undersized.jpg

    Measurements of pockets and inlays -
    001 - Pockets, inlays - measurements.jpg

    Using 2" as zero to test Y axis calibration -
    003 - Using 2 inch mark for zero to test Y calibration.jpg

    Moved 48" and this appears to be perfect -
    004 - Using 2 inch mark for zero and moving 48 inches to test Y calibration.jpg

    Using 2" as zero to test X axis calibration -
    005 - Using 2 inch mark for zero to test X calibration.jpg

    Moved 25.75" and this appears to be perfect -
    006 - Using 2 inch mark for zero and moving 25.75 inches to test X calibration.jpg

    Setup for X axis calibration -
    007 - Measuring X axis calibration.jpg

    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
    David
    CurlyWoodShop on Etsy, David Falkner on YouTube, difalkner on Instagram

  2. #2
    Join Date
    Apr 2017
    Location
    Tucson, Arizona
    Posts
    620
    So it looks like you machine is cutting 0.008" to 0.010" under size for these pockets and inserts (inlays). I assume that when you "calibrated" your machine over the longer distance to match your tape measure, you were adjusting the "turns ratio" for you controller. Just curious, what specific controller hardware/software package are you using?

    One way to compensate for this under size cutting is to adjust your cutter size (diameter) in Fusion 360. For example, if you want to increase the cut diameter of you round pocket by 0.010", then tell Fusion 360 that your cutter (endmill) is 0.010" smaller in diameter than what the setting is currently. This will cause Fusion 360 to compensate by moving the cut path 0.005" towards the outside of the pocket, resulting in a diameter increase of 0.010" (not taking into account the discrepancies caused by the grain orientation around the inside of the finished pocket).

    If you want increase the outside diameter of the round insert (inlay) by 0.010", then tell Fusion 360 that your cutter (endmill) is 0.010" larger in diameter than what the setting is currently. This will cause Fusion 360 to compensate by moving the tool path 0.005" towards the outside of the part, resulting in an outside diameter increase of 0.010" for the finished part.

    You could set up your tool table as Tool Number 1 and Tool Number 2, and set one for internal pockets and the other for the outer perimeter parts (inserts/inlays). You can still use the same physical endmill installed into your router/spindle.

    This would be my work-around to correct your dimensional issues for these particular parts. You may need to do something similar with larger parts. Without knowing more about your specific machine, construction, system backlash, etc. it would be hard for me to be more specific as to a recommendation as to where to start to track down the actual cause of your dimensional discrepancies.

    David





    Fusion 360 adjust cutter diameter.jpg

  3. #3
    Join Date
    Apr 2017
    Location
    Tucson, Arizona
    Posts
    620
    Have you measured the backlash in your x and y lead screws? If so, what were your results?
    David

  4. #4
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,772
    This sounds kind of familiar to a thread way back I think where you were having issues not cutting to size. Beyond the mechanical issues David mentions, Im assuming youve accurately checked that your tooling is cutting dead on size and not over/under cutting as well as tool/mechanical deflection differences on climb vs. conventional cuts, insde pockets vs. outside profiles?

    I think I remember saying in the last thread that this would bug me too as I would want super accuracy but one possible work around though it may not work if you have specific finished inlay dimensions to hit and a lot of stock removal after, is to move to a V inlay instead of a straight sided inlay if acceptable. That pretty much eliminates the few thou from the programmed dimensions as long as your machine isnt cutting over in x and under in y or some other combination due to the backlash or other issues.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  5. #5
    I have had similar issues with inlays. I have had the best results by creeping up on the final fit, using very slow feed rates to cut down on bit deflection. By cutting the male parts first, then cutting the pockets intentionally small and incrementally enlarging them by increasing the allowance in VCarve (or changing the bit size in the file) I can get close enough.

    It may be that there is enough bit deflection with small diameters or there is some backlash in the system that causes the discrepancies. It seems to me that if your calibration is rght on for large dimensions, the software is telling the cutter to follow the correct path and the problem is in the mechanics of the cut.

    I have not done any v inlays, but that is a suggestion worth trying- it should be more tolerant of small inaccuracies.

  6. #6
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    652
    Quote Originally Posted by David Buchhauser View Post
    So it looks like you machine is cutting 0.008" to 0.010" under size for these pockets and inserts (inlays). I assume that when you "calibrated" your machine over the longer distance to match your tape measure, you were adjusting the "turns ratio" for you controller. Just curious, what specific controller hardware/software package are you using?

    One way to compensate for this under size cutting is to adjust your cutter size (diameter) in Fusion 360. For example, if you want to increase the cut diameter of you round pocket by 0.010", then tell Fusion 360 that your cutter (endmill) is 0.010" smaller in diameter than what the setting is currently. This will cause Fusion 360 to compensate by moving the cut path 0.005" towards the outside of the pocket, resulting in a diameter increase of 0.010" (not taking into account the discrepancies caused by the grain orientation around the inside of the finished pocket).

    If you want increase the outside diameter of the round insert (inlay) by 0.010", then tell Fusion 360 that your cutter (endmill) is 0.010" larger in diameter than what the setting is currently. This will cause Fusion 360 to compensate by moving the tool path 0.005" towards the outside of the part, resulting in an outside diameter increase of 0.010" for the finished part.

    You could set up your tool table as Tool Number 1 and Tool Number 2, and set one for internal pockets and the other for the outer perimeter parts (inserts/inlays). You can still use the same physical endmill installed into your router/spindle.

    This would be my work-around to correct your dimensional issues for these particular parts. You may need to do something similar with larger parts. Without knowing more about your specific machine, construction, system backlash, etc. it would be hard for me to be more specific as to a recommendation as to where to start to track down the actual cause of your dimensional discrepancies.

    David

    Fusion 360 adjust cutter diameter.jpg
    I have considered manipulating the tool specs to achieve the results I want but I keep thinking there must be something else going on. And I have done this a couple of times in a pinch but I would rather figure it out (just me and the way my mind works... ugh! LOL!). I've also used 'Stock to Leave' and manipulated the final size that way.

    Quote Originally Posted by David Buchhauser View Post
    Have you measured the backlash in your x and y lead screws? If so, what were your results?
    David
    It's been a while, David. It's R&P and was on the low side, 0.001" to 0.002". Even if it has increased due to wear I don't think that explains why the pockets are smaller than they should be. If anything I would think they would be larger if there was significant backlash. Also, I can engrave very tiny letters and they are crisp and precise, so no indication of mechanical sloppiness is apparent.

    I 'snuck' up on this engraving to get the depth and look I wanted, seems like I lowered Z a couple of thousandths and ran this three times in total.
    004 - Romans 323 Trivet - Walnut - new logo.jpg

    Quote Originally Posted by Mark Bolton View Post
    This sounds kind of familiar to a thread way back I think where you were having issues not cutting to size. Beyond the mechanical issues David mentions, Im assuming youve accurately checked that your tooling is cutting dead on size and not over/under cutting as well as tool/mechanical deflection differences on climb vs. conventional cuts, insde pockets vs. outside profiles?

    I think I remember saying in the last thread that this would bug me too as I would want super accuracy but one possible work around though it may not work if you have specific finished inlay dimensions to hit and a lot of stock removal after, is to move to a V inlay instead of a straight sided inlay if acceptable. That pretty much eliminates the few thou from the programmed dimensions as long as your machine isnt cutting over in x and under in y or some other combination due to the backlash or other issues.
    Yes, Mark, I did have calibration issues a while back. But after calibrating to the larger dimension and squaring the gantry, which was the bigger issue at the time, all cuts seem to be exactly what I have specified in F360. Until, that is, I try to do some inlay work and find that pockets are undersize by enough that the inlay pieces won't fit, which are much closer to the specified size.

    I have thought about doing the V inlay but that's not always an option. I could probably do that and make it work most of the time but I really want to understand why I can cut larger pieces and they measure correctly but doing the small, intricate pieces don't.

    Quote Originally Posted by Kevin Jenness View Post
    I have had similar issues with inlays. I have had the best results by creeping up on the final fit, using very slow feed rates to cut down on bit deflection. By cutting the male parts first, then cutting the pockets intentionally small and incrementally enlarging them by increasing the allowance in VCarve (or changing the bit size in the file) I can get close enough.

    It may be that there is enough bit deflection with small diameters or there is some backlash in the system that causes the discrepancies. It seems to me that if your calibration is rght on for large dimensions, the software is telling the cutter to follow the correct path and the problem is in the mechanics of the cut.

    I have not done any v inlays, but that is a suggestion worth trying- it should be more tolerant of small inaccuracies.
    That's what I have been doing, Kevin. I cut the inlay pieces first and then use 'Stock to Leave' to creep up on the pockets until the inlay fits like I want. I just don't understand why I can cut a 10" or 16" or 26" Longworth chuck or any size in between and they come out exactly as I have specified. I cut some 3" discs recently and they came out within a couple of thousandths (gotta' remember I'm dealing with wood - haha!).

    As for deflection, that's why I take a rough cut in climb and leave 0.005" for a final clean up pass in conventional direction. I don't figure there's much deflection involved with taking 0.005". I could be wrong, of course, but I can see the final pass does cut. I have even run the toolpath a second time to see if it touches the sidewall for another thousandth or anywhere and it's a clean, no cut pass; doesn't touch the sidewall at all. So that, to me, rules out deflection.

    But if I cut a pocket of any size it's always small regardless of the size or shape. So what's the deal with pockets...? I don't get it and I truly hope it's something simple I have overlooked.

    David
    David
    CurlyWoodShop on Etsy, David Falkner on YouTube, difalkner on Instagram

  7. #7
    Join Date
    Sep 2006
    Location
    Deep South
    Posts
    3,911
    Are you sure it isn't flex in the gantry?

  8. #8
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    652
    Pretty sure it's not that, Art. It's a stout machine and we're talking about a 1/8" bit, actually 0.123". One reason I take the rough cut and leave 0.005" for a clean up pass is to rule out deflection, flex, fiber compression in the wood, etc. The final pass takes a mere 0.005" and I don't think that small amount would cause any of these issues. Plus, I have run the toolpath a second time to see if it cuts anything and it doesn't - it's an air pass.

    David
    David
    CurlyWoodShop on Etsy, David Falkner on YouTube, difalkner on Instagram

  9. #9
    Join Date
    Oct 2007
    Location
    Dawson Creek, BC
    Posts
    939
    8 - 10 thou is quite respectable for the machines in our class. Companies that do better than that use CMM equipment to setup their rails and gantry. You will also see how the machine startups differ. Many have a squaring routine where the machine checks all its dimensions multiple times when it starts up. Using those dimensions, it then compensates the values coming from the servos minute amounts. Now I am sure many will disagree on much of this, but I am skeptical unless images with calipers are included as well as the cutting specs. CNC accuracy discussions seem to be a bit like fish stories.

    I typically use a -0.010"+- on my tool path, but it takes a couple tries usually to get something I really like. I also find it can depend where you cut the parts. Backlash compensators need to know more about our machines than the our software usually includes. You can read all about their use on the practical machinist website where they take this topic to the next level.

    Here is an example cutout years ago I made when checking accuracy of my machine. Here I could easily measure the dimensions with 8" calipers. I eventually picked up a 24" set of calipers to check larger dimensions. This image was before I had found and corrected the initial setup problems.
    EXAMPLE.jpg
    Last edited by Brad Shipton; 01-31-2020 at 11:51 AM.

  10. #10
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,772
    I get caught in these tail spins all the time but then Im subscribed to channels like Edge Precision on youtube and I watch him creep up on a 2 thou part with a 150K Mazak and tooling and years of experience on petro and aerospace work. Its nothing to see those guys miss a mark (probably intentionally) by 5-10 thou over and then dial it in in one or two passes, but then we want to hit them in a single shot, in wood for goodness sake, and with a machine that is 1/20th the cost. :-)

    I am squarely in your camp. I know I could figure a work around but I would want to know why, and if I absolutely have no other option, than to use that workaround. I just often times dont have the time.

    Seems like it would come back to the old post. Clearly quantifying what dimension your tooling and machine is actually cutting on a given climb/conventional at a given load, then repeating those cuts on an inside pocket and outside profile, and then adjusting from there.

    I recently ran some super complex parts in solid surface that had to match dead nuts. I never thought it would happen and got behind scratching my head thinking it was never going to work and I was going to destroy 1K of material. And I guess Im just lucky to have a machine that when they came off they went together dry with an invisible seam. That said, this week plowing through melamine, you can clearly see tool deflection with a return onion skin in parts coming off. Small ridge on the return skin.

    There is a lot too this stuff, and Im constantly reminded that Im glad its wood an not a $20K Titanium blank Im responsible for.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  11. #11
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,772
    Quote Originally Posted by Brad Shipton View Post
    8 - 10 thou is quite respectable for the machines in our class. --- CNC accuracy discussions seem to be a bit like fish stories.

    Just an assumption (never good) but I think you experience with your machine biases you in some regard. My experience is no machine biased and may just be luck, luck in the machining, luck in the machine, but I am consistently able to blow my mind machining complex parts that make an 8-10 thou tolerance seem like a pot hole. The solid surface we ran recently for instance, your not going to get away with any visible gap when it gets seamed. The joints must be nearly invisible on dry fit. Thats not 2-3 thou. Thats invisible. And it blew my mind that they were. I'd never have believed it.

    Bottom line is, especially in wood, you know when your dead on, and you know when your not. When I measure a double sided laminate panel (not melamine, laminate), and run a dado pocket and its a press fit, and I kick the dado out 2 though and run it raw (not a spring pass) and its a perfect hand fit, I know Im pretty much running true.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  12. #12
    Join Date
    Oct 2007
    Location
    Dawson Creek, BC
    Posts
    939
    Mark, you would have to show me how you derived your figures as both our machines are built on the same frame using similar techniques. We are both interested in the fit, and I understand your argument, but we are talking figures and it is easy to throw out numbers that may or may not coincide with the reality of the materials we are working with. You have servos, and that will help as they will be correcting steps. Many in this group are using steppers like mine. For reference, I measured a sheet of 20lb piece of paper on my desk and it is 0.002". 0.005" is still quite a good fit, but I will agree that 0.010" is a tad ugly. I had a custom cutter head made for cope and stick. They used a 0.003" design gap for the stick profile, and that fit is very tight many days. I have done a better when machining aluminum parts that need to fit into something else, but I do so with cleanup passes. The big boy machines I got quotes from were in the realm of +-0.003" for accuracy, and they could actually measure that and put it in a quote. When questioned about that, they said they would need to know the ambient temperature and materials before they could talk about values less than that. The one supplier sells machines in the aerospace industry, so I am confident they know what they are talking about. Soilid surface material machines brilliantly.
    Last edited by Brad Shipton; 01-31-2020 at 12:43 PM.

  13. #13
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,772
    Quote Originally Posted by Brad Shipton View Post
    but I will agree that 0.010" is a tad ugly.
    .010 is beyond ugly when it really comes down to it. Its a pencil line. Again, these conversations swing to climate controlled clean rooms, isolated HEPA air, central chilled water cooling the machine ways and spindle, and then a 15-30-50K cnc slid into someones 2 car garage on the back of the local roll back wrecker service dripping oil all over your driveway... Its an unrealistic swing in comparison.

    Every time one of these pops up I kick myself in the #^@#$ for not taking a feeler gauge and spending 3 hours documenting on a post or youtube about the fit, but I have to make money, not content. The simple fact is these solid surface parts were complex cuts. Negatives cuts, angles, radius, masons miters, large pieces, and heart pounding the entire time and they were seamed together flawlessly immediately off the machine. Im not touting shop sabre in any way, Im without doubt camaster, or any other multitude of machines do it all day long in their sleep.

    My point is thinking that 8-10 is default in a sub 50K machine may not be very accurate though your stepper issue may play a pretty serious part.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  14. #14
    Join Date
    Oct 2007
    Location
    Dawson Creek, BC
    Posts
    939
    Mark, my point in mentioning the temperature control was not to suggest it was a consideration for our work, but rather to suggest that our material is not known to be stable or as consistent as others. Some of our materials don't even come supplied in consistent thicknesses, yet we use numbers to suggest perfection with respect to fit.

    Would 5-10thou be to your liking? Many suppliers skirt the discussion entirely. The sub 50k do not cut to the same accuracy as the 100k+. I appreciate the 100k are intended to cut much faster, but their parts, setups and the quality control at the fabrication stage are different in many respects. You have mentioned the 0.002" number a few times before and I have never followed your basis for the use of this figure. I was curious to understand where it came from many times before, but I never bothered to ask. I gathered the complex fit aspect of your parts and I am not disputing they fit perfectly. I am not sure it takes hours to measure, nor did I think there was a need for a video of some sort.

    By the way, I am not suggesting the .008" tolerance is reasonable stop point, but when I want to do better it takes some trial and error. It is annoying, but I have to live with it until I can replace a few more parts. I suspect we have all had to learn a lot of different things that are unique to our machines.
    Last edited by Brad Shipton; 01-31-2020 at 3:04 PM.

  15. #15
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,772
    Quote Originally Posted by Brad Shipton View Post
    You have mentioned the 0.002"
    I work harder at documenting.. Though I see a .0005 machine in your future with some form of adapted wood dust collection. lol. I know for a fact Im in the .005 range daily in a small format. Across 100 inches not so much.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •