Ovrclck350

04-27-2010, 08:33 AM

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

Thanks in advance.

Thanks in advance.

View Full Version : Quick G12.1 Question (L20)

Ovrclck350

04-27-2010, 08:33 AM

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

Thanks in advance.

Thanks in advance.

tejano4life72

04-27-2010, 11:57 AM

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

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

04-27-2010, 12:34 PM

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

Ovrclck350

04-27-2010, 02:34 PM

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]

Ex:

[G12.1 setup]

G0X-.3Y-.3

G1X-.2Y-.2

Y.2

X-.2

Y-.3

[RAPID OUT]

UK-Engineer

04-27-2010, 05:33 PM

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!

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

04-28-2010, 02:26 PM

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?

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!

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?

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!

Powered by vBulletin® Version 4.2.2 Copyright © 2019 vBulletin Solutions, Inc. All rights reserved.