I'm having problems getting my circles to be the correct size. My program is telling my machine to go 7.2mm dia but the circles the CNC is making are perfect little 6.99mm (maybe 7.0 when I push the calipers) dia. Machine travels x and y distances perfectly across 600mm, so I can't believe it's a problem with $100, $101, $102. What am I missing? I imagine for a larger circle this could be even further off.... Brand new Blackbox x32 put in place of my SparkConcepts V3 - same parts except the controller. The old Spark controller and configuration didn't have problems with circles. It must be something I setup in the config? Any ideas?
Is there any chance your endmill is slightly undersized? I measure all of mine with a digital caliper. I have received several from well known brands what were undersized. One was a 1/4" Freud that was actually 6.11mm in diameter across the cutters.
Measured it in fractions at 1/8, measured at 3.15mm, which is slightly smaller. Running a few tests right now.... 0.125 = 3.175; so 3.15-3.175 = 0.025; which doesn't really cover a 0.2 mm difference. That's still off by a factor of 10x.
Hm. Now I'm stumped. Adjusted the program to a 3.15 endmill and reran - worked, with reservations. I have since remeasured it using the thick part of the caliper closer to the readout - 3.17 is what it gives me. When I first measured it at the end of the caliper tip it was 3.15 so I think I just have a little flex in my caliper at the end. I validated this by testing a nut I have and at the tip it's off by 0.02mm but perfectly measured closer to the readout. So the endmill is in fact 3.17 which is about as close as I'm going to get to 1/8. While I don't think I have solved the problem, it seems I can just adjust the diameter of the bit to accommodate whatever my machine is doing wrong. So if it isn't the endmill, what else could it be?
The shaft may be correct, but the cutters may be slightly smaller. That seems to be the case for the cheap Chinese 3.175mm endmills. At least that has been my experience. I did have one surprise me the other day and be pretty much on the money. I put them in the caliper and rotate the backwards with the caliper closed until I see the largest reading across the cutters. I have that same caliper and I also noticed that the gap does not close completely along its length (not counting the notched out area) so I put a god amount of pressure on to zero it out. But it really only is off by 0.02mm for mine, so it isn't horrible. Apparently, Igaging is at least consistent with their error.
One problem I have found with 1/8 endmills is how much they flex when cutting. Have you tried cutting the item with a 1/4 inch? That may help narrow down if it is an endmill issue.
I make a lot of small holes for projects in plastic, wood, aluminum and G10, they are always undersize, it's a combo of flex and backlash. I adjust my drawing to give enough tolerance to make things work. As long as the location is good everything works out. Gary
Totally great advice. Changing my bit to a 3.15m (it's actually 3.17, aka: 1/8th, using the above-mentioned end mill size test) and running 3 passes over each important hole has been working. It feels like a terrible solution, but you are probably right. There's 0.5mm of flex in those bits and the only way to get it right is to go over it several times. When I'm done with this project I'll test with some high-quality bits that should be size-accurate and see if I can produce a circle of correct dimensions.
You could be buying OSG or Sandvik end mills and they'd still be undersize if they're not designated as "over-tolerance". When the carbide is sintered and centerless ground, it's made to around +0/-0.1mm tolerances. That's why "proper" machines have tool probes as well as work probes. Generally we have to measure offline as best we can, which is quite difficult with an odd number of flutes since you can't just throw it in a micrometer (and even then, it technically isn't absolute diameter, but widest single cutting edge radius that matters). The best I've come up with so far is a height gauge on a surface plate, which has gotten me perfectly adequate results in testing recently... (No, I don't expect to repeat that too often!) A roughing-finishing strategy, maybe a spring pass in some materials, and often a tool wear comp offset (not available in grbl, hence the lying to the computer about its diameter) is pretty standard in industry. Flex happens on every machine and every tool.
I agree with the roughing finishing pass I pretty much do that on everything now. Also, if the hole is 4.5 mm or greater, I will use a. 4mm endmill since they are 25ish percent more material so should be less flexible. I attempt to use as big as possible. I tracked down an 8mm collet for my RoutEr11 and had fun this weekend roughing out pockets at 15 mm deep and a 45% step over at 3000mm/min with an 8mm two flute.
I just found the automatic probe function in Control. First, way cool. Second, does anyone know if Interface will get the same feature? I hate bringing out my laptop for just that feature. That said, it doesn't seem to be very accurate even though it has the potential to be truly amazing. It checks in 6 directions the dimensions of the bit, and with me holding that probe perfectly steady, it came up with an even smaller bit. Other than being off, it entered the probe hole in the upper right so very close to the edge. If I had a 1/4 bit in there I bet it would have smashed it. LOVE the feature, hope it can have increased accuracy and adoption to Interface!!!
Two clues here Not entering the hole centered, and measured dimension reporting different from reality : both indicates the machine is moving more/less than it thinks it is! In other words, time to go to Wizards and Tools > Calibration and do it accurately (calipers, engineering rulers. Not a $1.50 class D measuring tape) and over maximum distance (you can enter own length to move)
I used a precise 600mm Shinwa H101-E ruler down the x and y axis. I setup a precision 1/2" brass depth block exactly at 600mm. Placed a blank probe in my router, moved the ruler to touch it. Increased z so it rose above the ruler then moved it exactly 600mm over so it was touching the brass block sitting at 600mm. I don't know how to get more accurate than that. No cheap rulers were involved. I promise I will record a video so you can see.
Probe video: Calibration video: It's almost like it centers itself where it's supposed to be hovering over 0,0,x, then jogs right and down. Rather than going down and slowly right.
What's this line of gcode doing in the macro? [00:48:05] [ G0 Z14 ] ok [00:48:05] [ G0 X0 Y0 ] ok [00:48:05] [ G0 X4 Y4 ] ok [00:48:05] [ G0 Z1 ] ok This happens just after it finds the X,Y zero. If I am reading the code right, after it finds the outer surface locations, it goes to the new X0/Y0 and Z 14mm above 0. Before it jogs down though into the hole, it jogs X4 Y4, then after the jog it drops to +1 above the new Z0. Was that intentional? To have it enter the hole from +4 on the X/Y axis? Maybe that's right, to get to the side faster? Was just odd to not see that bit go to Z1 first, and then jog to the side @F100 speed. The above sample video shows that jog at 28 seconds in.
New discovery as I was setting up my brand new CNC. The Shinwa H101-E, "high precision" ruler, isn't precise. Over 600 mm it's off by ~2 mm. I ended up using my higher precision (hopefully) iGauge and moved it 100mm using the calibration tool built into OpenControl. Adjusted and now it seems to be tracking correctly. I will cut a few holes and see if the problem is fully resolved, but the high-precision ruler might have been the main culprit after identifying the bits as not perfectly sized and the old CNC having too much deflection. I guess when I say it that way, pretty much everything was wrong. ..what's new.
