Newbie- Trying to write G-code to cut a tapered flute

[claires-dad]

Hi, I've built a CNC router to use for building a pinball machine. Most of the work is fairly straightforward using my 2.5D CAM program (Vectrix Cut2D), but I'm stuck on one cut. I need to cut a tapered flute at the bottom of the shooter lane. The cut should look like a cylinder intersecting a plane on an angle, or a groove with a rounded bottom where the depth varies. I thought I would cut it with a 1/4" ball-nozed end mill either of two ways: using G01 cuts parallel with the cylinder, or a sequence of G18 G02 cuts to cut cross-sections of the cylinder.

Has anyone done this before, or something similar? This is my first attempt at writing G-code beyond very simple scripts to test my machine, so I'd appreciate any suggestions or pointers. Thanks.

--Steve


Here's a picture - ignore the slot at the bottom, it's the angled flute that's the challenge.

[fordav11]

if your machine can handle the cutter you can use a large ball-nose slot drill or some kind of ball-nose router bit.
start the cut at one end and cut only in 2 axis X Z.
for example if the length of the slot is in the X axis something like this....

G00 X0 Y0
Z1.0
G1 Z0
G1 X15.0 Z-0.3


One cut and problem solved

I have one pinball machine. My slot is not very deep (~0.300) and is about 15" long.

The cutter doesn't really need to be any bigger than 1 1/8" to maybe 1 1/4" because a standard pinball is 1 1/16" diameter.

If you want to use a smaller cutter try to use the biggest possible so you will have less sanding of steps to do after.

To use my above method with smaller cutter do something like this....

G00 X0 Y0 (Y0 is middle of slot)
Z1.0
G1 Z0
G1 X15.0 Z-0.3
G0 Z0.1
X0
Y0.1 (*)
G1 Z0.05 (*)
G1 X15.0 Z-0.25 (*)
G0 Z0.1
X0
etc


The Y and Z sizes marked by * will need to be properly calculated to give a smooth curve with multiple passes.
It can be done using CAM software easily.

[claires-dad]

Thanks for the info. Unfortunately, I can't use that large a cutter. I had started with the CNC machine because I had been unable to find a 1-1/16" ball nose router bit. On my machine, I'm limited to cutters with a 1/8" or 1/4" shank.

Your second method is one I was planning to use - if anyone out there can suggest an algorithm for looping through the cuts, that would be great.

[fordav11]

To do it that way will require CAM software to get the curve smooth.

Your other method of multiple G02's will work if you can tilt and clamp the board to your required angle. It shouldn't be difficult just pack it up at one end with a approx. 0.200" spacer and clamp it down.

Then just do a heap of identical arcs in YZ plane. You don't even need to do any calculations. Just cut 9/16" rads (half of dia 1 1/16").
Set your Z0 to approx 0.36" above the top of the material and it will cut air for the first part. The depth at the deepest end will be around 0.200". If you need more taper increase the spacer packing.

example (in metric)

T01
M06
G54
G97 S1000 M3
G0 X0 Y13.49
Z0
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X1.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X2.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X3.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X4.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X5.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X6.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X7.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X8.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X9.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X10.0 Y13.49
G19 G02 Y-13.49 Z0 K0 J-13.49
G0 X11.0 Y13.49

etc


keep increasing X by 1.0 (or 0.5) and repeat the G02 line

see pic attached for a sample showing it works

[SquibLoad]

Originally Posted by claires-dad Thanks for the info. Unfortunately, I can't use that large a cutter. I had started with the CNC machine because I had been unable to find a 1-1/16" ball nose router bit. On my machine, I'm limited to cutters with a 1/8" or 1/4" shank. Your second method is one I was planning to use - if anyone out there can suggest an algorithm for looping through the cuts, that would be great.

Try these:

MLCS core box and round nose router bits

This should do the job. I've used these for large diameter relief cuts while making bridges for guitars, and they work well. Just raise (or drop) your Z from start to finish by an amount that matches the slope of your ramp. Quick and easy.

[SquibLoad]

Originally Posted by SquibLoad Try these: MLCS core box and round nose router bits This should do the job. I've used these for large diameter relief cuts while making bridges for guitars, and they work well. Just raise (or drop) your Z from start to finish by an amount that matches the slope of your ramp. Quick and easy.

Also forgot to mention that Whiteside will cut just about any bit you need.

Or, you could use an indexed tool holder and have a blade cut that matches the radius you need. Any local tool sharpener could cut one for you.

[fordav11]

they don't have 1 1/16" in 1/4" shank. its not practical to have a small shank and big cutter head.
the above program will work with a smaller cutter then he can just sand it a bit to smooth it out (or take smaller steps)

[claires-dad]

Thanks for the program example. I get confused easily with G02/G03 in a different axis, so this helps and should do the job.