A month or two ago, in anticipation of future projects, I bought
myself a High-Z/S-400T CNC milling machine from cnc-step.de. While
waiting for my next lathe to arrive in order to complete the Stirling Engine,
I had a go at my first milling project, which I decided would be a
maze cut into brass plate. Saffron Walden is a maze town (it has
three and runs a maze festival every few years) so a maze seemed
appropriate. The object created is not meant to be for
anything in particular, more an exercise in learning how to use
the machine and associated software.
First I went to www.mazegenerator.net
and generated myself a maze. I went for 20 by 20 hexagonal
cells (which looks quite pretty) and iterated, changing the E and
R values and looking at the solution, until I had something which
used most of the maze and had plenty of dead ends (i.e. low E and
low R):
Then I saved the result, one with and one without the solution
shown, as PNG files. I did try saving to SVG file first but
the SVG file you get is made up of many small vectors which
doesn't work readily with a CNC application (which needs closed
shapes in order to understand how to mill them):
For the CNC side, I used VCarve Pro from Vectric. I imported the
PNG file and used the trace function to draw a closed vector
around the bitmap image.
The effect I would like to achieve is for the maze shape to be
milled into a brass plate. The problem with the closed shape
I have achieved above is that the application thinks I want to
mill inside the border walls instead of between
them. To fix this I used node editing to split the single
closed vector at the entrance and exit to the maze and close just
the inner vector on itself, deleting the outer vector
entirely. I also turned the entrance and exit points into
pleasing circles, adding an inner circle to each that can be
milled to a different depth, potentially providing a "home"
position for a small ball-bearing. Here is the result:
Taking these vectors and cutting a 3 mm deep slot with a 2 mm end
mill produced the following simulated result inside VCarve Pro:
nbsp;
I saved the resulting toolpaths to a format which my CNC milling
machine understands (the one for a WinPC-USB controller) and
milled the pattern onto a piece of MDF to test things out; the
extremely fuzzy video is speeded up 64 times to roughly match
the simulation speed above:
nbsp;
The MDF was only loosely held as I discovered I didn't have some
of the clamping pieces required, so some misalignment was to be
expected, however what I didn't understand was why some of
the areas where the software had chosen to plunge in (before later
drawing out the maze proper) were considerably deeper than the
areas where it simply cut out the maze (see lower left in the
picture below):
There's no sign of this in the simulation. I did pause
somewhere between the plunging and routing phases in order to
re-charge the battery in the camera and I think I heard an unusual
noise from the machine when I did so, so maybe that was it?
I'll need to try it again to be certain.
My next clever idea was to cut the maze in perspex. What I
hadn't anticipated was that the milling tool would get so hot when
digging the furrow that it would melt the perspex, resulting in
this horrible mess:
nbsp;
I should have taken several passes at it.
Enough messing around, I need to bite the bullet and cut into
brass now. Taking into account various resource around the
internet, I chose a 2 mm two-flute end-mill, a tool speed of
20,000 RPM, a feed rate of 4 mm/second, a plunge rate of
0.3 mm/second and a pass depth of 0.3 mm. This results
in an estimated total milling time of four hours
(10 passes required) for a 3 mm final depth of cut.
Maybe I should have chosen something a lot simpler to mill on my
first attempt, especially as the WinPC-USB software's USB
interface has crashed and lost contact with the machine during
each of my test runs?
Since I must wait a few weeks for some very cheap ["H62", 343-460
N/mm2 tensile strength] pre-cut brass plate to arrive
from China, I milled this toolpath (though with the tool only
running at 3500 RPM) into a spare perspex sheet to check the
quality of such a long run and the real duration. Nine hours later
(i.e. just under an hour per pass) here's the very pleasing
result:
No crashes occurred: I had
the USB interface plugged directly into the PC rather than through
a [powered] USB hub; so maybe that made the difference? And there
was no loss of registration over the nine hours of travel; look at
the sides of the maze above, those are cut in ten passes with
never a return to reference position and yet there is no sign of
stepping. Very impressive. The only thing I would like
to improve is the scuffing on the surface (see Note On Terminology at the
bottom of this page). Asking at www.mycncuk.com I was moved
to purchase an end-mill with a radiused corner (0.2 mm) to
reduce the scuffing. It was also suggested that the tool
speed in perspex should be more like 8000 RPM and I was
pointed towards a very useful web-based calculator for CNC milling
parameters FSWizard.
While waiting I ordered a pack of 2 mm stainless steel ball
bearings from e-bay; these worked nicely in the perspex maze.
For the final cut in brass I increased the depth of the maze
slightly (final depth of cut 3.8 mm now,
13 passes). I polished the top and filed down the sides
of the brass plate, then began milling.
nbsp;
10 hours into the job the milling bit began making a screeching
noise and, on the final pass, it broke off. You can see from
this picture, compared with an unused bit, that half of the tip is
missing and it is clogged with brass:
Now, since the milling did not finish, unevenness in the base can
be expected (in that it had drilled some clean-out areas and not
yet milled across that part of the pocket) but, even taking that
into account, the damage at the end of the bit has cleary had an
effect on the bottom of the cut, which seems somewhat smeared, and
on the walls, which have steps in them:
I was driving the bit too hard. The specified cutting depth
for the bit was 3 mm, though measured it looked more like
4 mm so I went with my 3.8 mm final depth of cut but
maybe I was over-egging it and the bit overheated rubbing against
the walls in the last few passes? I revisited www.mycncuk.com to ask for
more advice, where I learned:
the downloadable Windows application version of FSWizard,
HSM Advisor, is well worth
purchasing as it has many more features, like estimating how
hard you are pushing the milling bit,
the sticky-outness of the tool from the collet has a large
impact on how much material you can remove at a time and how
long the tool will last; my sticky-out-ness was 20 mm
(because I am cutting close to the edge of the material and
have to get the collet nut over the clamps) which is high but
not terrible,
with this small a carbide bit, cutting in brass, just go
for max RPM,
consider keeping the last 0.1 mm as a separate pass,
possibly with a brand new tool to achieve the best possible
finish,
HSS tools are sharper than carbide tools and so can be run
at a lower RPM; carbide tools last longer if they are treated
well but are more inclined to break and must be run at a high
RPM (because they are not so sharp), hence they can get hot
and this leads to clogging of the tool or smearing of the
surface on soft materials such as brass,
cooling the milling bit by blowing air directly at
the cut can give a significant improvement in cutting quality
and tool life.
I should try something on the last point but it looks complex, so
I tried a HSS tool first and ran it at a lower RPM: a 4 flute
HSS, 8% cobalt, end-mill (4 flutes as I couldn't find a
2 mm diameter two flute HSS end-mill, though I later learned
that a slot-mill is the same thing*),
no shoulder radius this time (as I couldn't find a radiused HSS
tool of 2 mm diameter either), 7 mm flute length and
with a 6 mm diameter shaft for additional strength. I
ran it at half the feed-rate that HSM Advisor suggests, so just
5 mm/second, and the motor was running at
14000 RPM. HSM Advisor reckoned I could cut 0.8 mm
depths at a time but I reduced to 0.5 mm. I also kept a
final pass of just 0.1 mm depth as a separate CNC file so that I
could run it with a fresh tool if the first tool seemed damaged
after its exertions.
And, wouldn't you know it, despite a very good looking cut, after
not even one lap the bit snapped:
nbsp;
It looks as though the tips of the milling bit have worn rather
quickly (circled above) and then it has become clogged with
brass. I returned to a www.mycncuk.com
for yet more advice. Most observers seemed to think that I
shouldn't be having so much trouble but, with such a long cut for
the maze, cooling and removing chips, so that they don't end up
clogging things, are wise moves.
I learned a HUGE lesson while changing tools at this point: do NOT
put the movable tool length sensor that comes with your machine
underneath your park position. While that seems logical, if
you accidentally leave it there and press "start", depending on
how the Z clearance is set up for your job, the tool may come down
and slam into the length sensor, destroying £200 of sensor.
Instead, put the length sensor in a location that you would not
normally move the machine to. And, as a matter of procedure,
ALWAYS move the sensor out of the way after use. Thinking
about it, it seems odd that the tool should come down first and
then move into X/Y position, that's more likely to hit something
isn't it? Ah well.
Next, I made myself an air cooler. I bought a small Jun-Air
compressor off e-bay, a solenoid valve, a pressure adjusting
valve, some 1 mm internal diameter copper pipe to form a jet,
various adapters/tubing and a sheet of aluminium to make a mount
for the milling machine.
I returned to two flutes (which, advice suggests, is better) and
thought I'd try a PM60 "Only One" end mill (just for variety) that
is definitely capable of a 4 mm deep cut, run at 1400 RPM. I
only turned on the cooling air during the long slot-cutting runs
and for occasional bursts to clear out chips as my Jun-Ar
compressor (model 6-25) motor likes to have 15 minute breaks
between runs; using 2 bar pressure of pressure for a good air jet
means more like 2 minutes on to 4 minutes off. Part of the
way through the cutting I noticed that there was a vibration while
side-milling at one end of the brass plate; I think the plate was
not completely flat and so wouldn't clamp against the surface in
all places. The vibration was sufficient to shove the
cutting bit up into the collet by about 1 mm. Not wanting to
unclamp the piece and lose registration I tightened the bit,
forced some old feeler gauges that I use for packing into the
gaps, re-measured the bit length and continued the cut. I
might consider putting some cushioning beneath the piece in future
to absorb any vibration.
nbsp;
Anyway, hey presto, it is done! The cut is of good quality
(compare it with the perspex
above); cooling is the thing.
Oh, and the tool tip was worn but not damaged, no sign of melted
brass. Cooling is definitely the thing.
Here are the files as used: the VCarve
file, and the main and final NC files.
* A NOTE ON TERMINOLOGY: a
"slot" mill, originally called a "slot drill" is good at cutting
vertically downwards while an "end" mill is not intended
to cut vertically downwards but it is intended to mill
across its bottom face. Both are able to cut on the side.
Hence you can use a slot mill/drill to cut vertically downwards
and then along but the finish on the bottom of the slot will not
be so good while an end mill will create a good finish on the
bottom of the slot but you can't cut straight downwards, you have
to "climb" or "ramp" into the cut. I only found this out after
finishing the above, so ideally what I should have done is made
the final cut with an end mill to achieve a good finish on the
bottom of the maze (since the files I used always climbed into the
cut in any case). Back to Meades Family Homepage
