Cutter accuracy

[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.

[Paul3112]

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

[komatias]

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

[Neale]

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.

[magicniner]

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.

[Neale]

I take your point, but I am taking light cuts off MDF (a 1mm pass, 4mm depth of cut, 6mm cutter). I'm not saying I'm right, but I can't see how I can take cuts much lighter than that! I'm only removing dust at this point.

[magicniner]

If your cut errors are consistent then you can use cutter compensation to correct for the mysterious error you are encountering.
If you want to locate the error and the cutters are not under size by the error you are seeing then something on your machine is flexing by close to the error amount, there is no magic by which a cutting edge can temporarily shift into another dimension to allow the edge to dodge the material ;-)

[Neale]

To draw a line under this one (at least, until something else makes me get out the worry beads)...

After doing a lot of checking, measuring everything I could, including duplicating measurements I had already done, I have concluded:

my X ballscrews (2005, C7) appear to have a pitch error of about 0.1mm in 100mm. This is somewhat greater than the nominal C7 accuracy of 50um in 300mm, and I would put it down to measuring error except that...

my Y ballscrew (1605, C7) appears to have a similar error but in the opposite direction. I would like to measure travel over a longer distance but I'm limited by the measuring tools I have available (Mitutoyo 200mm vernier caliper, in this case).

Both these errors could be compensated by tweaking "steps per" in Mach3 although I'm a little reluctant to do this without being able to check errors over a larger range.

All ballscrews seem to have about 50um backlash. I have not been able to find a spec for this for a C7 ballscrew, but it's a bit more than I would have hoped. However, for a machine intended for mainly woodworking, this is perfectly adequate, and even for making things like profiled aluminium plates isn't an issue. However, I might consider carefully doing things like machining a bearing housing and that might still have to be done on the milling machine with a boring head or suchlike.

Rechecking cutter diameters, I think that my original problem was that my single-flute cutters are cutting a tad undersize and I shall need to go through and carefully check and record actual cutting sizes so that I can include these in my CAM tool library. I note comments about tool tables, but on the whole I prefer to work with a "calibrated" tool library in CAM and not bother with tool tables in Mach3. I might change my preference in time (I have used tool tables with LinuxCNC in the past - I'm happy with the principle) but the net effect is the same. I have control of the whole CAD/CAM/CNC cycle and I'm not in a production environment where a machine operator will update tool tables locally due to wear/tool change or whatever without needing to re-CAM the part.

Thanks for all the comments, guys, but I have been suffering from my usual position that I don't quite trust anything that I have built while placing too much confidence in bought-in components!