[ajclay]

I'm always behind the times. I just heard about cutting internal threads with a milling machine. I've got a CNC Wells Index with Mach3 as the controller.

Can someone point me in the right direction on how to research the operation? It may not be possible with the machine and controller I have.

How is the code/program generated?

I'm not sure I'm even using the right name.

Any and all help is appreciated.

Thanks, Aj

[Geof]

The machine needs to be able to do helical interpolation. That is moving the Z axis up or down while doing a circle using G02 or G03.

Then it is simply a matter of programming the correct radius circle with the Z movement equal to the pitch of the thread.

[Caprirs]

You machine has to be capable of helical interpolation to perform thread milling operations.

Code is the same as circular interpolation except a Z is added along with a P. The Z is the end position of the helix and the P is the number of "paths" or circles the cutter has to make.

Thread milling starts with the hole at drilled/bored to the minor diameter.

So thread milling a 1/4-20 internal thread 1/2" deep would look something like this:

G0 X0. Y0. (move to center)
Z.025
G1 Z-.500 F20. (start at bottom to climb mill)
X.0321 (move tool to engage, depends on major dia. of thread milling tool)
G3 X.0312 Y0. Z0. I-.0312 P10. (moves up .500" in 10 circles =.05" pitch)
G0 Z.025

The above works for a single point thread milling tool.

If the tool has a longer length of cut, it is possible to cut all the threads in a single path/circle, move to center, and retract:

G0 X0. Y0.
Z.025
G1 Z-.500 F20.
X.0321 (depends on major dia. of thread milling tool)
G3 X.0312 Y0. Z-.450 I-.0312 P1
G1 X0. Y0.
G0 Z.025

The P and Z must obviously be matched based on the pitch of the thread.

Thread milling allows even tiny benchtop machines to create big threads. In addition, thread milling allows for more precise control of the pitch diameter which can be handy if the part eventually will get plated or anodized.

[ajclay]

Caprirs, you make it sound so simple. I have a basic understanding of g-code. Enough to trouble shoot my posts that are made with sheetcam. I don't know if I could handle that code all from scratch.

I machine is capable of 3D work, so it's got to be able to do circular interpolation ,but my brain isn't quite there....

Are there any programs out there that's capable of generating the g-code with the proper inputs? tpi, tool offsets, diameters, ect.....

thanks, AJ

[Geof]

He hit you with a lot in a big lump, take it in bite size pieces. Programming a circle is easy and to make it easier let's ignore the fact that the tool has a diameter(radius) and just look at the path of the centerline of the tool with the work zero at the center of the circle.

Now if you want to have the machine describe a 2" diameter circle (1" radius of course) you move either X or Y to a position 1" away from the work zero.

N1 G00 X0. Y1.0 (Line numbers are just for reference)

Now to program the circle you just use the G02 or G03 command with I and J

N2 G03 I0. J-1.

Depending on the machine/controller this command may be slightly different. My machines interpret the I value and the J value as the distance from the tool position to the center of the circle. In line N1 I did not move the X axis but I moved Y + 1. inch so therefore the center is -1. away from the tool position.

Line N2 tells the machine to do one circle. Some machines allow you to put a L (P) command to do multiple circles and line N3 would do three circles.

N3 G03 I0. J-1. L3

If the machine will not permit the L command it is necessary to program the necessary number of circles as in N4 thru N6.

N4 G03 I0. J-1.
N5 G03 I0. J-1.
N6 G03 I0. J-1.

Now if you can get the machine to move in the Z direction you have helical interpolation, which can be used for boring a hole by moving Z a small amount during each circle, or milling a thread by moving it the lead of the thread for each circle.

Again it depends on the machine/controller and the simplest is when the machine can perform an incremental Z movement while it is doing the circle. With this the command to spiral down three circles at 10tpi is:

N7 G91 G03 I0. J-1. Z-0.1 L3

When this type of command is not allowed it is necessary to do it the long way. Starting at the Z0. position the commands to do the same thing as line N7 are:

N8 G03 I0. J-1. Z-0.1
N9 G03 I0. J-1. Z-0.2
N10 G03 I0. J-1. Z-0.3

That is the basic idea behind thread milling.

Naturally you do have to take into acount the cutting diameter of the tool and this is done using tool compensation, the best method, or calculating the radius to correct for it, very tedious. Also when doind an internal thread you need to have moves to allow the cutter to enter gently into the cut, not just slam straight in on a radial motion. These are details you can learn once you are familar with the basics.

Write a bit of code and cut some air at very slow feed rates so you can see what is happening.

[ajclay]

[QUOTE=Geof;925593]He hit you with a lot in a big lump, take it in bite size pieces. Programming a circle is easy and to make it easier let's ignore the fact that the tool has a diameter(radius) and just look at the path of the centerline of the tool with the work zero at the center of the circle.QUOTE]

Thank you for taking time to explain further. I'm going to do a little studying on what you lined out. It's going a day or so to soak in...

Thanks, Aj

[robertproff]

Thread mills usa has a free excel file for programming a thread mill. All you have to do is change the parameters (thread dia., cutter dia, tpi, thread depth, sfm, feed per tooth, and # of flutes) and it will give you program for thread milling. This is very useful until you become more familiar with thread milling.
Threadmills USA - Programming Help