| The first question that most people
ask when using carbide mini and micro tools to cut wood (and other soft
materials) for the first time, is, "What are the best speeds and feeds?".
What they really want to know is, "How fast I can cut without breaking a
bit? What are the optimum cutting conditions with my equipment?"
As with most things in life, a precise answer to
these questions is usually very difficult to come by. However, there are a
few techniques that one can use to determine a very good approximation to
the ideal conditions for machining the material at hand.
The following discussion assumes that you have
measured the runout (TIR) of
your spindle and found it to be less than 0.001" (0.025mm), that your
spindle bore and collet / tool holder have been
cleaned with ColletCare and, finally,
that the backlash on both the X and Y axes of your CNC router are less
than 0.001" (0.025mm).
In any material, tool performance, and longevity
are primarily influenced by:
- feedrate ramp or acceleration
- feedrate
- spindle RPM
Acceleration
Acceleration is defined as the rate that a
velocity changes. The acceleration that we are most concerned with is
how fast an XY movement goes from 0 to the selected feedrate (F) once the
computer tells the controller to move. In the graph below, the
acceleration (also known as ΔV/ΔT) is the slope of the ramp of the red
velocity plot. The steeper the ramp (higher acceleration), the quicker the
axes get up to speed. The shallower the ramp (low acceleration), the
longer it takes to get to "F".
 20 inches per
second per second, or
0.51m per second per second
your bit will think that you are
coddling it like a wee little baby and not break as soon as it starts to
move. This is especially important as the bit starts to get dull and
cutting resistance increases. Of course, if you set the feedrate (F) too
high, the rupture point will eventually be exceeded and the bit will break
anyway, but more about this in a moment.
Feedrate and Spindle RPM
We consider the feedrate (FEED) and
the spindle RPM (SPEED) together because, in the case of cutting soft
materials like wood and plastic, it is their combination into a single
parameter known as "CHIP LOAD" that matters the most. As the name
suggests, chip load is the amount of material (load) each flute cuts
during each revolution (every chip). Another way of looking at it is how far
the bits chews into the material every time it rotates one full turn.
As the chip load increases (deeper
penetration per revolution), the transverse stress on the tool
increases. Clearly it is important to keep the stress below the breaking
point of the tool. On the other hand, at very low chip loads, not much material is being cut
so there is nothing to carry heat away from the bit. Below a certain
limit, the tools gets too hot and abrasion rolls away the cutting edge,
rendering the bit useless.
There is another aspect to chip load that is often overlooked. As the bit
turns and starts to cut, material "flows" across the outside and inside faces
of the cutting flutes. If this material "flow" is too high on the outer
surface (low chip load) the cutting edge rounds over. It the material
"flow" is too high on the inner surface (high chip load) the cutting
debris cannot be evacuated quickly enough causing it to back up and pack.
With nowhere to go, the impacted material seals off the flute and the bit
breaks. When the outside and inside "flow rates" are balanced, edge
erosion is symmetric and the bit stays sharper longer. We call this the
"sweet spot" What we need to do is find
this magical point where feed
and speed are balanced in such a way to provide optimum cooling, and
balanced material flow to maintain the sharpness and integrity of the
cutting edges. Happily, in the case of many soft materials, this is
relatively simple to do. The figure below shows a simple pattern that can
be used to derive the optimum machining parameters for any combination
of wood and cutting tool.
The program is quite simple.
- A set of parallel slots 1" long are spaced
apart 3 times the diameter of the bit that you are
testing (S = 3 X Bit dia.)
- For a given RPM (SPEED), an initial
feedrate (FEED) is chosen so that the bit cuts 0.0005" per
revolution. For example, if your speed is 20,000 RPM then a feed of
10 IPM (inches per minute) will yield a full bit chip load of
0.0005"/rev. (just divide the feed by the speed).
- Plunge as deep as you intend to cut and
make the first 1" slot.
- Pick up the tool, move to the top of next
slot.
- Increase the feed by 1" (25mm) per minute.
- Cut the second slot.
- Pick up the tool, move to the top of next
slot.
- Again increase the feed by 1" (25mm) per minute.
- Continue in this fashion until one of two
things occurs. Either the bit will break or the quality of the
cut will markedly deteriorate.
- Whichever happens, stop the test and
record the feedrate where the bit started to fail.
- Multiply this value by 0.75 to get the
sweet spot for these cutting conditions.
Schematically the cut sequence would like
something like:
"BREAK THE BIT? Are you out of your mind?" you
scream. Well, maybe a little bit, but not in the way that you mean. The
reason for this test is to show that the optimum cutting point is MUCH
closer to bit breakage than it is to the point where the feed is so low
that friction from the spinning bit actually burns the wood. The good news is that,
once you have done this a couple of times with different diameters and a
variety of materials, you will be able to calculate the approximate the
sweet spot for any other bit / material combination. But that is a topic
for another tutorial.
Todd Reith (Reith Guitars) offers a very valid objection to this testing scenario. He
points out that lifting the tool between each cut does not accurately
reflect the cutting dynamics encountered in most machining
operations. He proposes the alternate cutting plan comprising:
- A set of parallel slots 1" long spaced
apart 3 times the diameter of the bit that you are
testing (S = 3 X Bit dia.)
- For a given RPM (SPEED), an initial feedrate
(FEED) is chosen so that the bit cuts 0.0005" per revolution. For
example, if your speed is 20,000 RPM then a feed of 10 IPM (inches per
minute) will yield a full bit chip load of 0.0005"/rev. (just divide the
feed by the speed).
- Plunge as deep as you intend to cut and make
the first 1" slot.
- Cut to the right a distance equal to S.
- Increase the feed by 1" (25mm) per minute.
- Cut the second slot.
- Cut to the right a distance equal to S.
- Again increase the feed by 1" (25mm) per minute.
- Continue in this fashion until one of two
things occurs. Either the bit will break or the quality of the cut
will markedly deteriorate.
- Whichever happens, stop the test and
record the feedrate where the bit started to fail.
- Multiply this value by 0.75 to get the sweet
spot for these cutting conditions.
 |
