G12/G13 Circular pocket help needed

[NeoMoses]

I want to use the G12/13 circular pocketing in Mach2, but I can't find any good documentation on the arguments. Can anyone give me a hand?

[Paul_S]

I'm not familar with the Mach2 mill. The Haas mill uses G12/G13 for c'bores The syntax being G13 I(radius value) F(feed rate) [L (number times)]

G13 is counter clock wise - climb cut
G12 is clock wise - conventional cut

If the codes have a syntax for circular pockets. There should be a variable/G word for step over or for tool radius.

The Fadal control uses an L subprogram instead of G12/G13. And variables R0 and R1 for c'bores L9400 ccw and L9500 for cw. R0+(feed rate value) R1+(diameter) The L9800 ccw would be the pocket routine were R0+(feed rate) R1+(tool radius) R2+(diameter)

Write a sample program using G13 I.5 F2. D(tool dia offset being used) and see if that does a 1.00 id c'bore. If that doesn't work try a J or an R or an X until you find the correct G word for the radius. If the word is for a dia it will of course cut 2x as big.

If the G13 I F D format works just using it as a c'bore command you can use it to do pockets too.

G1 Z-.125 F2.
G13 I.25 F2. D01 (first cut)
G13 I.375 F2.5 (first step)
G13 I.5 F5. (last step)
G13 I.5 F23. L2 (finish spring passes)
G0 Z0.1

I'm not saying that it must be done just that way. Just an expample of how it could be done. (The feed and speeds, of course, need to be calculated for the materal, tool size, and finish.)

I hope this was useful. (I didn't see any other replies.)

[tobyaxis]

This isn't a Mach 3 Manual but it might help you to understand the Concept of Spiral, Helical, and Circular Interpolation.

Go to this website and download the Yasnac MX1 Operators Manual.

http://www.yaskawa.com/site/Support....ucts%20Defined

[psychomill]

Both Toby and Paul covered a good part of the answer but to add to them...

I as well don't use Mach software but keep this in mind. It also depends on the coding that Mach is similar to and borrows from. As Paul states, using G12/13 would work that way... however, provided that your control actually has G12/13 as valid G codes. For example, the codes work on in that manner on Haas and Yasnac controls. But, it doesn't work on FANUC controls (unless added by the machine builder). You either need a ladder program or a macro program to use it. There are many examples of G12/13 programs written as macro sub calls for FANUC. The common code usage is G112 and G113 though (in many cases... not always).

Here's an example of a "G12" custom macro... by Mike Lynch I believe. This is just one version. There are many. You can (again, not sure on Mach) set up this program to use a "custom G code" by setting parameters for it (like using G112 or G113 instead of G65).

[ger21]

In Mach3, G12/G13 are not circular pockets, but just plain circles.

[tobyaxis]

Originally Posted by ger21 In Mach3, G12/G13 are not circular pockets, but just plain circles.

G2/G3 can do that, why is Mach 3 using G12/G13???
This is why I tell people that most CNC Controls are different to a degree.

[ger21]

It's a simple circle with center and radius. Sort of a "canned" circle. G2 and G3 work fine as well.

[tobyaxis]

Originally Posted by ger21 It's a simple circle with center and radius. Sort of a "canned" circle. G2 and G3 work fine as well.

Can it do this??

[texaspyro]

Originally Posted by psychomill But, it doesn't work on FANUC controls (unless added by the machine builder).

Reviving a thread from the dead...

Many Fanuc machines do have a circle command. They Use G12.2 and G13.2

Their lead-in and lead-out cuts are a bit different. Fanuc leads in with a 45 degree linear cut then does a quarter-circle arc to the edge of the main circle (abd thre reverse on the way out) Most other machines do a full 180 degree lead-in/lead-out arc. Mach3 just does a horizontal linear cut to the edge.

Fanuc and Mitsubishi the only machines that I have seen that that support circle operations (not to be confused with G02/G03 arcs) in planes other than the G17 XY plane.