Cutter accuracy

Been trying out my new CNC router with a few simple jobs. Trying to cut slots in thin ply, I found that my cutter seemed to cut consistently under size. 3mm single-flute cutter gave 2.6mm slot, or equivalent result cutting opposite sides of plain block (I.e. block was oversize after cutting by same amount). Tried a couple of other single-flute cutters (4mm and 6mm) which also seem to cut about 0.4mm undersize. Difficult to directly measure diameter of these cutters, but putting the 6mm cutter along a straightedge, the tip does sit slightly below the line of the shank. Is this normal? Do I need to, in effect, calibrate the diameter of a cutter before using? Are 2-flute cutters more accurate?

Which software are you using and in which mode do you see the error? I mean constant velocity or exact stop mode or both consistently? New cutter with 0.4mm error in 3mm is a lot, but I have received cutters with that much error from the factory, brand new. Of course, cheap eBay stuff but I complained and the seller sent me a batch of new ones and those were good. I don't know if 2-flute cutters are more accurate than single flute, but I guess they are easier to make and to measure, so I prefer using 2-flute or more, but I don't cut ply or any other wood.

I was using Mach3 via my CSMIO IP/M. However, CV or exact stop was not relevant here because for my test pieces I was typing gcode directly into the MDI window and just taking straight cuts. For testing, I fixed a blank to the spoil board and took a straight cut down each side. I moved the cutter sideways by a standard amount (54mm in this case) between cuts. I was taking very light cuts so do not believe that cutter deflection was an issue. What I expected to measure between the cut faces was 54mm minus cutter diameter. I actually measure 54mm minus cutter diameter plus about 0.4mm.

I do not believe that it is machine calibration error as I did these tests immediately after doing a gantry squaring test. This involved drilling 4 holes at the corners of a 100mm square, putting the shanks of new drills in the holes, and measuring diagonals. However, as a cross-check I also measured the sides of the square (all four sides) and saw consistent and accurate measurements to generally better than 0.1mm.

I was using cutters from a couple of UK sources. The own-brand 3mm cutter from CNCRouterShop is quite old now but my old router had so much play in every joint that I could never work to this kind of accuracy, so can't tell if it was like it from new. The 4mm and 6mm cutters are own-brand from Regal and are brand new.

Hi Neale,

Just to check, if you plunge down and just drill a hole, then drop the shank end of a 3mm drill in does it fit? If not does a 2.5mm one fit? That would tell you the diameter of the cutter. If that is off then you will just tell the CAM software the true diameter of the tool (i.e. 2.6mm) and all will be well again.

Thanks for the suggestion. Checked 3/4/6mm cutters and all make accurate size holes. Checked backlash with dial gauge - approx 0.05mm on X axis. Accuracy otherwise better than 0.01mm over 10mm (dial gauge range). Also used 6mm cutter to make two holes 150mm apart, push drills into holes and measure with vernier calipers - around 0.05mm errors. Tried moving gantry to include/exclude backlash just to make sure - no obvious issues. So happy with Mach3 "steps per" settings. Clamped block of MDF to bed and machined both sides and measured. Light cuts (1mm or so, DOC 4mm, 6mm cutter, so no cutter deflection expected). Comes out approx 0.3mm oversize.

So, not much backlash, spindle positioning good, cutters make true size holes. But machine does not make accurate cuts. Baffled.

Normally cutters when new are spot on. Even Chinese. Check size though before inputting in CAM.


next step is 30mm circle in say 50mm square. 1mm depth, best i use Phenolic sheet as its very precise and holds incredible detail, same time not affected by temperature or humidity. As MDf is not right even 1 min after the cut/ i live near the sea.



If problems like in your case, then i go even simpler and do pure straight lines. dig 1mm deep and tell mach3 or controller to move 20mm. Then line will be 20+d of bit, easily measured with caliper. So its easy to figure whats happening and where.

Quote:

---

Originally Posted by Boyan Silyavski

Normally cutters when new are spot on. Even Chinese. Check size though before inputting in CAM.


next step is 30mm circle in say 50mm square. 1mm depth, best i use Phenolic sheet as its very precise and holds incredible detail, same time not affected by temperature or humidity. As MDf is not right even 1 min after the cut/ i live near the sea.



If problems like in your case, then i go even simpler and do pure straight lines. dig 1mm deep and tell mach3 or controller to move 20mm. Then line will be 20+d of bit, easily measured with caliper. So its easy to figure whats happening and where.

---

Hi,

Cutting oversize ? If I read and understand correctly.
I would have a go at the step per given movement in Mach3.
Having said that i would also suggest that you do it over 85-90 % of axis travel
The quick and dirty way is the 3 4 5 triangle ( some maths involved to be within the limits of the shortest axis travel) but as big as you can get.
we mark out on a 3mm mdf fixed to the table and pin in tool on the spindle. does not have to be in the spindle , I have used darning needles fixed to the z axis. as long as it is constant position. Align the MDF to the long axis, errors will be the the diagonal and y axis
the test here is to see how close the DRO is to the measured distance marks. any variance in the x and y units will show up in the diagonal.
Regarding tool dia. Mach will let you put anything into the tool library for a tool dia. To me this this is the width of cut, the end of the day when of the all run-outs have had the effect. ( now having said, that I assume that the z axis is true perpendicular to both x and y .. it will effect the cut profile). I use off-cuts of corian I get it from the off cuts bin at the kitchen counter top factory. The bits they cut out for the sinks.
When swinging the z axis the bigger the radius the better. At this stage one can see if the x axis (for the purpose of this chat .. the long axis) are running parallel and flat to the bed. just move it to the corners of the bed at a fixed z height. If its out try jacking up the corner of the frame and leave it for a day. the colder the slower it beds it self in. A machinist level is the tool here level the x axis rails then the Y axis.
Sorry for the ramble, Public holiday afternoon here with a kit shelving job in progress lubricated with a very nice single malt.

Regards
Paul

Neale,

Most solid carbide cutters I have used are undersized by a little bit. The deviation you describe, I agree is a bit large.

Assuming that your machine is set up correctly:

You need to learn to use the cutter compensation function to be able to tweak the final finishing pass. Remember to set the tool table up and also tell you CAM program to set compensation in the controller and not computer.

Kind regards

Paul, Boyan - thanks for the comments.

To clarify:

Steps per in Mach3 is set to the correct calculated value for the ballscrew lead and microstep settings on my machine. Assuming that the ballscrew is to spec (and it is only C7), any significant error is due to a mechanical fault, which is what I am trying to find. However, over a short distance (up to 10mm, the range of my dial gauge) travel error is down around the 0.01mm region. Over 150mm, measured using two holes plunged with a 6mm single-flute cutter and measuring across two drill shanks pushed into these holes, travel error is around 0.03mm but this is measured with a vernier caliper so not as accurate as the dial gauge. All movements are designed to allow for backlash. If I repeat any of these checks with gantry movements arranged to maximise backlash, I see around 0.05mm error. I'm reasonably happy with these numbers for the moment.

I can plunge-cut holes with a number of different cutters and check hole diameter using drill shanks. All cutters seem to give correct sizes.

If I now take cuts on opposite sides of a (roughly 50mm) block to produce two parallel faces and measure them, there is a consistent error of about 0.3mm. Even though I have checked machine movement and cutter diameter.

All movements are single axis move and are done using manual gcode typed into MDI window, so CV etc corrections are not relevant. All movements are done at G1 rather than full rapid feed rate to avoid any possible missed steps.

Gantry squaring is not an issue here as I am just using movement in x axis (gantry move, the long axis, on my machine). However, I have set up squaring using the "4 holes in a square and measure diagonals" method and it's as close as I can get using vernier caliper to measure. It would have to be a long way off to generate the errors I see in the parallel-cut test.

If I put a dial gauge fixed to bed against the shank of a cutter held in the spindle and pull and push the gantry, I see a range of about 0.04mm - lost movement/backlash in overall system. There's a bit of flex as well if I lean on it hard enough, of course, but that's the figure for light loads. Dial gauge on shank and rotate spindle shows about 0.03mm TIR - collet error, probably.

So, I'm seeing reasonably accurate machine movements. I'm using cutters which appear to cut to size. When I combine these two, there is a significant error. I'm missing something really obvious here.

Overnight musing came up with the idea of positioning for my parallel cuts as above and trying to measure gantry movement to double-check this value under the same conditions as the parallel cut test. I'm trying to systematically narrow down the fault here, but running out of ideas.

Quote:

---

Originally Posted by Neale

If I now take cuts on opposite sides of a (roughly 50mm) block to produce two parallel faces and measure them, there is a consistent error of about 0.3mm. Even though I have checked machine movement and cutter diameter.

---

Try that with machinable wax or another material not strong enough to flex your machine's structure, there is a strong possibility that your machine is flexing under the forces applied by the test cuts.