Page 1 of 5 12345 LastLast
Results 1 to 15 of 61

Thread: Calibration question

  1. #1
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    890

    Calibration question

    My calibration still isn’t as close as I know it can be so I created a file today for some testing and calibration. This is a busy piece but served its purpose. Here’s what I cut with a 1/4" two-flute downcut spiral bit running 18k rpm and 125 ipm. The depth of cut is 0.1875" and it is cut with one pass leaving 0.005" on the side walls for a final clean up cut to get the fuzz off. The depth needed to be just deep enough to allow my dial calipers in for good measurement.

    Calibration test - 8-11-18.jpg

    I started on the bottom left, ‘Before’, and made my first cut. You can see it was out +0.005” on Y and -0.010” on X. I changed the settings in Mach4 and then ran the top left. Ignore the diagonals, those are to ensure I didn’t get too close to the screws. The circled dimensions are exactly as they’re supposed to be. I then ran the top right and it’s exact on Y and out +0.005” on X. The middle right was next and you can see it is exact on Y but out -0.002” on X. Bottom right is exact on X and +0.005” on Y (I wrote it wrong on the piece). The circle is very close, as well.

    However, all of the inside circles are 0.015” to 0.025” undersize and I don’t get that. The outside squares, rectangles, and circles are close enough to be acceptable. I think the variance is due to the material which is a sort of soft Purebond plywood from Home Depot. If I was cutting hardwood I think the tolerances would be much closer.

    So how do I get the inside circles to cut accurately? This makes it very difficult when I’m doing inlays and inserts, fitting dowels or bolts in holes, etc. I can’t change settings now or the other measurements will be off and I don’t want that. Is it something not set correctly in Fusion 360? Something in Mach4? It's not mechanical; the machine is a Saturn 2x4 from Fine Line Automation and is very rigid and tight and if it was mechanical the squares, rectangles, and outside circles would be off, as well.

    Thanks!

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

  2. #2
    David, take this from someone who has never ran a CNC before. If you are cutting the outside of the rectangle or circles first, could something be shifting or could the file not be taking some measurement accurately post cut of the outside.

  3. #3
    Join Date
    Oct 2009
    Location
    Marquette, MI USA
    Posts
    519
    David...
    Before you can calibrate via your methods you will have to eliminate some variables first. The most overlooked are machine deflection and bit diameter. Cut outside of a 4" square, 60 ipm 1/8" deep, 15k rpm with a 1/4" bit. Cut it climb and conventional. Measure the dimensions. Conventional should be slightly smaller, but whats important is that HALF the difference is your deflection at .002 chipload. Now cut it at 180ipm and see if there is a difference at .006 chipload.

    Next measure the width of the slot cut by the bit for each case. That is the diameter the bit cuts. May in most cases, be different that the advertised diameter.

    These two tests allow you to be aware of the environment, not the accuracy. To check and verify if the step resolution is accurate you need a good eyeball, a sharp V bit and a precision rule. If you have one, like me, I like to use a USB microscope with crosshairs and a precision steel rule, but a vbit and a tape measure will work fine. Stretch the tape out in the X axis, align the vbit EXACTLY to a line for 1 or 2" and tape it down. Zero that axis. For a 4' machine I will command X to move 44" and see if I am exactly on the line for 44" plus what had been cut for zero.

    If not exact, using the keyboard in incremental jog mode, adjust the vbit to the proper mark with care and record the X position on the DRO. To adjust Divide the value in the DRO by the actual distance (tape) and multiply that by the current resolution number. Edit the rez number, reboot if needed and retest. Repeat for the Y axis.

    You want to do this over as long of a distance as is possible to minimize any human eyeball errors. .005 in 1" is vastly different than .005 in 40 inches.
    Gary Campbell
    CNC Replacement & Upgrade Controllers
    Custom 9012 Centroid ATC

  4. #4
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    890
    Quote Originally Posted by Bryan Lisowski View Post
    David, take this from someone who has never ran a CNC before. If you are cutting the outside of the rectangle or circles first, could something be shifting or could the file not be taking some measurement accurately post cut of the outside.
    Thanks, Bryan, but the board is securely screwed down to the spoilboard. It's not going anywhere.

    Quote Originally Posted by Gary Campbell View Post
    David...
    Before you can calibrate via your methods you will have to eliminate some variables first. The most overlooked are machine deflection and bit diameter. Cut outside of a 4" square, 60 ipm 1/8" deep, 15k rpm with a 1/4" bit. Cut it climb and conventional. Measure the dimensions. Conventional should be slightly smaller, but whats important is that HALF the difference is your deflection at .002 chipload. Now cut it at 180ipm and see if there is a difference at .006 chipload. I'll have to try this.

    Next measure the width of the slot cut by the bit for each case. That is the diameter the bit cuts. May in most cases, be different that the advertised diameter.

    These two tests allow you to be aware of the environment, not the accuracy. To check and verify if the step resolution is accurate you need a good eyeball, a sharp V bit and a precision rule. If you have one, like me, I like to use a USB microscope with crosshairs and a precision steel rule, but a vbit and a tape measure will work fine. Stretch the tape out in the X axis, align the vbit EXACTLY to a line for 1 or 2" and tape it down. Zero that axis. For a 4' machine I will command X to move 44" and see if I am exactly on the line for 44" plus what had been cut for zero. I'll have to see which tape 'appears' to be the most accurate.

    If not exact, using the keyboard in incremental jog mode, adjust the vbit to the proper mark with care and record the X position on the DRO. To adjust Divide the value in the DRO by the actual distance (tape) and multiply that by the current resolution number. Edit the rez number, reboot if needed and retest. Repeat for the Y axis.

    You want to do this over as long of a distance as is possible to minimize any human eyeball errors. .005 in 1" is vastly different than .005 in 40 inches. About 6 months ago I did something similar for measuring longer distance but must have missed something. I realize 0.005" over 40 inches is far better than 0.005" in 1 inch and that's what I'd love to see but I question how accurate my tapes are. I'll pull them all out to 48" and see how they compare.
    I checked the bit - it is 0.250" on the nose. If I really work at it I can make it be 0.2495" at the very tip of the bit but for all practical purposes, and for this test, it's a 1/4" bit.

    I know using hardwood or acrylic would be better but until I get this a lot closer I don't want to waste good materials. Because the X and Y are very close now I need to figure out what's going on with the inside dimensions. I can slow the feed rate but I don't really think that's the issue. And going from conventional to climb (or vice versa) won't amount to the 0.020" and greater errors I'm seeing. And if the X and Y are as close as they are I don't think any error in the R&P factors in on the inside dimensions.

    I have Forstner bits of the size holes I cut and I can't get those bits into the holes. I can accurately measure the Forstner bits and most are about 0.010" undersize but even at that they won't fit into the holes I'm boring, so that tells me my inside measurements aren't too far off.

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

  5. #5
    I hate guessing at responses but could backlash be an issue? Im no machine builder but when I saw all the varied measures on your test piece it just to me spoke to something transient/random-ish. This makes me want to run one of these on our machine.

    I regularly machine fixture pockets and then parts for a snug/press fit and its always johnny on the spot. Part of me would be scared to run one of these as I'd likely wind up flipping out.

  6. #6
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    890
    Quote Originally Posted by Mark Bolton View Post
    I hate guessing at responses but could backlash be an issue? I'm no machine builder but when I saw all the varied measures on your test piece it just to me spoke to something transient/random-ish. This makes me want to run one of these on our machine.

    I regularly machine fixture pockets and then parts for a snug/press fit and its always johnny on the spot. Part of me would be scared to run one of these as I'd likely wind up flipping out.
    I haven't seen any indication of backlash, Mark. The machine obviously has a little - I don't think you can build a R&P machine without a tiny bit. But it hasn't shown up anywhere else except when I try to do pockets and inlays. I can go to zero and run any of the cuts again and the bit doesn't remove any new material. That tells me the backlash, if any, is very tiny and not a factor and that the machine repeatability is very good. Even the inside cuts - no new material removed. If it kept removing material then I would just run the finish cut twice but that also tells me there's no deflection on the finish cut. But I didn't expect any, after all I'm only removing 0.005" in the finishing pass so I doubt the machine would deflect on a cut that light in softer material.

    Did you see the Command Chief Stripes plaque I did last week? That's what brought all this up; I have another one to do and the inserts or inlay pieces didn't fit precisely on the first one. I want to avoid the handwork again because I'll have more of these to do. I also want to do inlay work on guitars, like the one I just finished in the photo below, and if the inlay pieces don't fit then I might as well cut them by hand. But that's one reason I built the CNC is to do inlay work.

    036 - Command Chief Stripes, Walnut, Maple.jpg

    037 - Command Chief Stripes, size comparison.jpg

    The fact that the outside cuts are within a couple of thousandths to me is more the softer material I'm using rather than the machine. I may be in denial but I don't want to waste good hardwoods or acrylic until I get this much closer on the inside circles. Then I'll switch to some Walnut or Maple and do similar tests to really fine tune.

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

  7. #7
    Now I want to run one of these and measure lol

  8. #8
    Join Date
    Oct 2009
    Location
    Marquette, MI USA
    Posts
    519
    David...
    You appear to be falling into the "denial trap". Which means, You are assuming everything that has been accomplished prior was and even worse, is still right on the money. No amount of parameter adjustment will do any good if the machine isn't right and tight. To measure if there is backlash, use a dial indicator affixed to the table and bumping all axes, one at a time.

    You also say the bit is ".250 on the nose" Did you measure the slot that the bit was cutting as I instructed, or did you mistakenly measure the bit?
    Gary Campbell
    CNC Replacement & Upgrade Controllers
    Custom 9012 Centroid ATC

  9. #9
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    890
    Quote Originally Posted by Gary Campbell View Post
    David...
    You appear to be falling into the "denial trap". Which means, You are assuming everything that has been accomplished prior was and even worse, is still right on the money. No amount of parameter adjustment will do any good if the machine isn't right and tight. To measure if there is backlash, use a dial indicator affixed to the table and bumping all axes, one at a time.

    You also say the bit is ".250 on the nose" Did you measure the slot that the bit was cutting as I instructed, or did you mistakenly measure the bit?
    Haha! Denial trap is an easy one in which to fall, Gary! Part of that is because this is Sunday and I've been at church most of the day, no time to get out to the shop. And part of that is because the repeatability is so good. So to check backlash I can certainly affix a dial indicator to the table but what am I looking for when I bump each axis? I assume it should be run very slow and just bump it... I guess a better question is can you point me to a good procedure for checking backlash?

    No, I only measured the bit itself. Again, because I've been at church most of the day. I'll have to do that tomorrow and see what size slot it cuts.

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

  10. #10
    With all of my tools new or freshly sharpened i run a few cuts at depth/feed/speed and then measure the actual width if the cur and that's the value I put in for cutter diameter

    My thinking of backlash was only because on the test piece your spot on in some areas and not on the other side. I'm a machine noob though and watching your build as it went along clear you know your machine far more intimately than I know mine.

    I'm both eager and scared to run one of these in the morning lol.

  11. #11
    Join Date
    Jan 2012
    Location
    NW Louisiana
    Posts
    890
    I just made a pass 0.200" deep with the same 1/4" bit I used on the test and it cuts a slot exactly 0.250" wide. I have a piece of tool steel that measures 0.250" and it fits into the slot with the lightest of pressure. I also have a ground tool steel round piece that measures 0.249" and it drops in with even lighter pressure (I'm not forcing either one, in other words).

    Cutter width exactly 0.250 inch - 8-13-18.jpg

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

  12. #12
    I just ran the test cuts and will upload photo shortly.

  13. #13
    Here was my go in MDF. I dont trust the internal measures with calipers. Cant really get them in there very well and the sharp edges on the internals dont ever give me a positive feel. I should have pocketed the internals out and measured with a snap gauge. The 1.75 measure on the internal core of the circle was a mis-measure for me. That should have been the internal measure of the pocketed hole measuring 2.5" so 1.7405+twice the bit diameter would have been

    testcuts2.jpg

    I would think your dial indicator backlash test would be mag base indicator, bring gantry to the indicator and pre-load, zero indicator, put your machine in .001" jog mode and jog the opposite Y at .001 per click and see how many clicks for the indicator to move? Then same for the X. I have never done it on our machine.
    Last edited by Mark Bolton; 08-13-2018 at 11:04 AM.

  14. #14
    I see two issues here, when you command 1" or 12" of movement, are you really getting that movement. Second issue is backlash in the system, we won't even get into machine rigidity yet.

    First thing to check is to see if you are getting the proper commanded movement. I do this on CNC mills and you have a certain number of pulses per inch that have to be calculated based on your resolver/encoder count, ball screw or rack pitch and any gear reduction in the drive system. I use machinists gage blocks or 123 blocks stacked together to get a reasonable distance, say 6 to 12". You zero your indicator on one end and then command say 6" of movement and have a block sticking up on the opposite end so you are coming at the indicator from the same direction and see if your command of 6" actually get's you 6". You need to do this on all three axis of your machine.

    Then you need to check and see if you have backlash. Put your indicator on the spindle and touch a block on the table. Zero the indicator approaching say from the positive direction. then put your mpg in the smallest resolution you have, I do .0001" and dial the opposite direction until the indicator first starts to move, that amount is your backlash. You should have backlash tables in the control where you can enter these values.

    Do all of that and you should gain some ground on accuracy and size.
    Brian Lamb
    Lamb Tool Works, Custom tools for woodworkers
    Equipment: Felder KF700 and AD741, Milltronics CNC Mill, Universal Laser X-600

  15. #15
    Tossed a mag base on Y for the heck of it to see and while its pretty consistent there most definitely are a few tenths here and there in the .001 jog. I dont have a very good mag base and its just a cheap indicator. The first jogs are of course in .001 then the next are with .010 jogs.

    https://drive.google.com/open?id=16L...U0TqyqJ-WE-L8I

Posting Permissions

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