Quick G12.1 Question (L20)

[Ovrclck350]

When programming in G12.1 from the 30-Tools are both the X and Y dimensions still in diameter?

Thanks in advance.

[tejano4life72]

Straight out of WinCNC:

G12.1- (option)Converts C axis degrees and X axis movement to work like
a milling machine. Program X-Y axis and the control converts all the
commands to degrees automatically. X and Y are programmed in radius
values and zero is at the center of the part, like a milling machine.
Tool nose rad comp is also needed to use G12.1 correctly. Thinking
about the direction for G2/G3 and G41/G42 is backwards! You have to
imagine you are back behind the guide bushing looking to the cutter.
If you can't do this, then just do everything opposite!

There are some new options while calling G12.1. We used to have to
change parameters to use G12.1 #1125 Mill_AX and #1126 MillC , now
we can set these while calling G12.1 . See also G16 below.

G12.1 (no arguments uses C commands same as G12.1 D1 E=C)

G12.1 D0 E=C

D0 -You can use "C" or "Y" as the virtual axis while in G12.1
The manual suggests using "D1" to use "C" but I don't agree.
If in G17 X-Y plane, then I suggest you use "D0" to use Y".
Your choice, it makes no difference which you use! If D is
not on the G12.1 line then "C" is default.
Always have "D" first on the G12.1 line!

E=C -This will set the axis number of the system to use as the
polar axis. This depends if you are using the gang plate in
$1 or the U121B option in $2 or $3. Setting E=C will set the
proper axis automatically. If you don't use E=C on the line then
$1 C axis is default. For safety, always use E=C


(MILL A .3 SQUARE WITH .02R CORNERS)
T1100(Live face mill/.25" cutter /1/2"bar)
(M5)
M18C0
G98M59S3=1200 (GSE1110 is reverse rotation)
(G4)
M132(Y axis mirror image off) (if not T11-13 then M132 not needed)
G0X.8Z.1T10
G12.1 D0 E=C
G17
G41G0X.15Y.3
G1Y-.15,R.02F8.(or use G2)
X-.15,R.02
Y.15,R.02
X.15,R.02
Y.1
G40G0X.4Y0
G13.1
G18G99M60
M131(Y axis mirror image on) (if not T11-13 then M132 not needed)

G13.1- reverses G12.1 by setting control of the C axis back to C and H

G16- Plane select Y-Z cylindrical machining. To use this plane you need the
option of G12.1 milling interpolation. G16 is used to convert polar
C axis degrees to linear Y when machining "J" slots or cylindrical
cams. Most of these part prints are dimensioned with linear and radial
values, not degrees. Also the prints usually show the part cut and
spread flat. Radii are hard to program and adjust without G16 and tool
nose radius comp. G41-G42. Programming would be linear "Z Y".
The polar "C" axis is converted to a linear "Y" axis. Another use of G16
is to chamfer a cross hole equaly all the way around the hole.

G16C.15
C= Position of X axis to calculate from if the actual cutting
position is different. This is in radial value. C.15 = X.3

(MILL A J SLOT Sample program not tested yet but should work)
T900(.125" cutter / 1/2"bar/ to cut .156 slot)
(M5)
M18C0
G98M58S3=2500
(G4)
(M132 is needed to swap Y mirror image if using T1100-T1300)
G50W-.59
G0X.6Z-.1T9
X.3(to depth of J slot)
G12.1 D0 E=C
G16 (C.15)
G41G1Z-.02Y.078F6.
G1Z.1,R.02(or use G2)
Y.187
G3Z.256K.078
G1Y-.078,R.078
Z-.02
G13.1
G40G0X.6Y0
G50W.59
G18G99M20M60
(M131 is needed to swap Y mirror image back if using T1100-T1300)

G17- Plane select X-Y
G18- Plane select X-Z normally used. G18 is when power on.
G19- Plane select Y-Z

[cogsman1]

ALL values are in RADIUS until you cancel with G13.1

[Ovrclck350]

So, if I were to want to mill a square with zero chamfer, would the R-value offset still work?

Ex:

[G12.1 setup]

G0X-.3Y-.3
G1X-.2Y-.2
Y.2
X-.2
Y-.3
[RAPID OUT]

[UK-Engineer]

As others have said all dimensions are radial.

Also G2 and G3 radius are the wrong way round - machine looks at it from spindle perspective - clockwise is G3

R value in Tdata will work with 0 as P value for tool shape.

,R and , C will also work - A for angle doesn't

If we assume a square on centre with dimension of 1/2" AF then assuming you use X as vertical with C being horizontal your co-ors from top right hand corner would be

X0.25 C0.25 - Top right
X-0.25 C0.25 - Bottom right
X-0.25 C-0.25 - Bottom Left
X0.25 C-0.25 - Top left

Your code for L20 would be something like below - other methods are possible - it just depends on your preference

G42 is traversing clockwise around outside of shape

M25 G98
M174 S7=2000 (face power tool fwd)
T3200
(M118)
M48 C0
G0 Z-1.0
G12.1
G17
G42 G0 X0.9 C0.25 T32 (position above top right in X - allow for tool size)
G1 Z* F* (feed to depth)
X -0.25 (feed to bottom right)
C-0.25(feed to bottom left)
X0.25(feed to top left)
C0.35(feed past top right)
Z-2.0(tool clear)
G40(cancel comp)
G13.1 (Cancel Interpolation mode)
G18(reset plane)
G0 U0 Z-1.0 T0
M79 M176 G99
M119

good luck!

[Ovrclck350]

Thanks UK.

Just to clarify 2 points.

1. I can specify Y instead of C, correct?
2. If I understood you correctly, the R-value can still be used as an offset to adjust for tool wear as the tool wears as long as the P-data is set as P0. Is this correct?

Originally Posted by UK-Engineer As others have said all dimensions are radial. Also G2 and G3 radius are the wrong way round - machine looks at it from spindle perspective - clockwise is G3 R value in Tdata will work with 0 as P value for tool shape. ,R and , C will also work - A for angle doesn't If we assume a square on centre with dimension of 1/2" AF then assuming you use X as vertical with C being horizontal your co-ors from top right hand corner would be X0.25 C0.25 - Top right X-0.25 C0.25 - Bottom right X-0.25 C-0.25 - Bottom Left X0.25 C-0.25 - Top left Your code for L20 would be something like below - other methods are possible - it just depends on your preference G42 is traversing clockwise around outside of shape M25 G98 M174 S7=2000 (face power tool fwd) T3200 (M118) M48 C0 G0 Z-1.0 G12.1 G17 G42 G0 X0.9 C0.25 T32 (position above top right in X - allow for tool size) G1 Z* F* (feed to depth) X -0.25 (feed to bottom right) C-0.25(feed to bottom left) X0.25(feed to top left) C0.35(feed past top right) Z-2.0(tool clear) G40(cancel comp) G13.1 (Cancel Interpolation mode) G18(reset plane) G0 U0 Z-1.0 T0 M79 M176 G99 M119 good luck!