On Fri, Sep 8, 2017, at 02:19 PM, Gene Heskett wrote: > Greetings all; > > > I have measured the x axis of this lathe quite a few times, and arrived > at an X scale that moves it 1.000 inches according to a dial indicator. > > However, when carving metal it doesn't seem to be correct. > Part of the problem is almost certainly the difference between unloaded moves and loaded (cutting) moves. Tools flex, toolposts flex, machine flexes, etc.
When you are trying to set the "scale" of an axis, you want to use the longest travel that you can accurately measure. That minimizes the effect of things like lash, flex, etc. You can't consider the scale on an axis to be correct until you can command multiple different moves and have them all be correct. Command a 0.1", and the dial indicator better say 0.100". Command a 1" move, and the dial indicator better say 1.000". Command a 6" move, and dial calipers or indicator plus a 6" gage block or whatever you can come up with better say 6.000". And you should be able to make and measure a whole sequence of 1.000" moves all the way down the length of your axis. > For instance, the motor pulley I took off the OEM 3/4 horse has a .750" > bore, but the 1 hp motor on it now has a 7/8" (.875") OD shaft, and a > nominally 1" larger pitch diameter, so I undertook to bore the OEM > pulley to .875" yesterday, by first boring it out what I thought > was .1000", which should have taken it out to .850". But I didn't > get .850", more like .824". And had to make about 6 more swags to > actually get it to fit the spare, identical motor. There are probably two things at play here - flex and touch-off error. (Scale error could be happening too, but IMHO you shouldn't cut metal until you've verified scale with multiple measurements as described above.) I find it hard to do a really accurate touch-off on the inside of a bore. And even on the outside (where I gradually back the tool away from the part until a 0.250" dowel pin slips thru the gap), the touch-off is done with no load on the tool and is subject to change due to flex. In your situation, I would do the following: 1) Bring the tool into the 0.750" nominal old bore until it just takes a tiny chip. Touch off X to a radius of 0.375, diameter 0.750. I know this is probably wrong, but it gets me close. 2) Set X to 0.385 (0.010 depth of cut), which should give me a diameter of 0.770. Take a cut on the bore. Get the tool clear and measure the bore as accurately as I can (bore gage, telescoping gage and mic, whatever). That measurement tells me what the machine will do when cutting 0.010 deep. It will be different for heavier or lighter cuts, but I'm planning to finish my job with a 0.010" cut. 3) Reposition the tool back to X = 0.385 (using MDI). Use the touch-off button to reset the diameter to the exact measured bore diameter. Now I'm corrected for flex and anything else, and as long as the tool doesn't wear or something else bad happen I should be good. 4) Make roughing cuts at whatever depth of cut I can do until I get close. Final roughing cut should be at X = 0.4137, that is 0.020 (two passes) undersize on the radius. Measuring the bore after the last roughing cut isn't critical, but I usually do it just as a check. 5) Make my first finishing cut, with X = 0.4275, target diameter is 0.855". This cut is 0.010" deep, just like my calibration cut, so the flex should be the same and it should come out pretty darn close. 6) Measure the bore as accurately as I can. This one really counts. Maybe the tool wore a bit during roughing, maybe something moved, or maybe the flex or screw error is different since we're at a different spot on the axis. This measurement will let me fix that. 7) Move X to 0.4275, exactly where it was when I made the cut. If the measured diameter isn't exactly 0.855", hit the touch off button and set X to exactly half of the _measured_ diameter. This should set me up for exactly one more pass, cutting 0.010, which should have the same flex and everything else as the previous pass. 8) Make my final finishing cut, with X = 0.4375, target diameter 0.875. 9) Measure and hope I didn't screw it up. This procedure is NOT appropriate for production - I stopped and measured twice during the job, and probably modified the g-code a couple times (in some cases I don't even bother with a program except for the roughing, I make the first and final cuts with MDI). But for a one-off like Gene is describing, I've found this process to be the best way to get the diameter I'm aiming for. -- John Kasunich [email protected] ------------------------------------------------------------------------------ Check out the vibrant tech community on one of the world's most engaging tech sites, Slashdot.org! http://sdm.link/slashdot _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
