[slowdigits2]

i have a part i want to cut out its a simple rectangle 16"X7" its coming out of a pc round pipe its actually the hole that i leave is what i need but because of the radius my head will jamb and i need to cut on the z axis on a 9.625"pc of round (radius 4.8125") is there an easy formula and do i have to use adifferent command because im cutting the radius on the Z plane? apperciate any and all help i have what i think is the close gcode minus the radius caculations any feed back would be great THIS IS WHAT I HAVE BUT IT STILL CUTS THE RAD ON THE X Y INSTEAD OF THE YZ THIS IS ON A MAZAK 420 VCS CNC
thanks in advance.


G17 G20 G40 G80
G90 G54
M6 T3
M3 S1550
G0 Z0.8 M08
G90 G0 X8. Y-3.25
D2 Z-0.875 F5.
G1 G41 X-8. Y-3.25
G1 G2 Y-3.25 Y3.25 R4.8125
G17
G1 X8. Y3.25
G1 G2Y3.25 Y-3.25 R4.8125
G17
G1X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
G90
M30

[jeffrey001]

G17 tell the machine you are cutting on the X and Y axis.

Do a search with G18 and G19

Jeff

[MetalCarpenter]

Use g19 to arc in yz axis.use ijk when programming radius is my suggestion not R...trust me.k is center of arc in
Z axis, j is center of arc in y axis.

[slowdigits2]

THANKS FOR YOUR HELP Jeffery the picture heped a great deal but im having problems understanding the i,j,k were and how to use it this is what i have it runs with no errors but it just cuts the rectangle and will not cut the arc the white area in the image is what im trying to cut out but it wont follow the radius of the pipe .
thanks again for your help

Attachment 266542
G17 G20 G40 G80
G90 G54
M6 T3
M3 S1550
G0 X8. Y-3.25
G0 Z0 1. M08
G90 G0 X8. Y-3.25 Z-1.875 F5.
G1 X-8. Y-3.25 F20.
G1 G19 y3.25 J6.5. K4.8125
G1 G17 X8. Y3.25
G1 G19 y-3.25 J6.5 K4.8125
G1 G17 X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
G90
M30

[MetalCarpenter]

you need g02 g03 in there instead of g01 on the lines with the plane change code (g19). i dont know off the top of my head which will arc to z positive.try it above the part first.

if your at x1.0 and want to arc to x-1.0 the I is 0 because the center of the arc is at x0. if your at x6.0 and want to arc to x4.0 the I would be 5.0. thats a one inch radius in this example fyi not accounting for tool diameter. just the movements.

[silverslammer]

your code looks like you're defining the j+k in absolute mode, most machines are incremental from the start point.

[silverslammer]

metalcarpenter is absolutely correct....need g2/g3 's

[silverslammer]

try this:
G17 G20 G40 G80
G90 G54
M6 T3
M3 S1550
G0 X8. Y-3.25
G0 Z0 1. M08
G90 G0 X8. Y-3.25 Z-1.875 F5.
G1 X-8. Y-3.25 F20.
G3 G19 y3.25 J3.25 K1.5625
G1 G17 X8. Y3.25
G2 G19 y-3.25 J-3.25 K1.5625
G1 G17 X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
G90
M30

[slowdigits2]

sorry just having a hard time with this i didnt think it would be this hard or its just my old brain lol thanks aga guys

[slowdigits2]

try this:
G17 G20 G40 G80
G90 G54
M6 T3
M3 S1550
G0 X8. Y-3.25
G0 Z0 1. M08
G90 G0 X8. Y-3.25 Z-1.875 F5.
G1 X-8. Y-3.25 F20.
G3 G19 y3.25 J3.25 K1.5625
G1 G17 X8. Y3.25
G2 G19 y-3.25 J-3.25 K1.5625
G1 G17 X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
M30

i tried this silverslammer i get an 806 illegal address (rad, 0 , 9) at G3 G19 y3.25 J3.25 K1.5625

[silverslammer]

its probably the "k" value i gave you....you don't need the 'I" value since you're not moving on "x"....do you know if your IJK's are suppose to be absolute? usually they're incremental from the start point, having said this i have seen them as absolute...just not very often.....you can try a simple arc move, just do it in the G17 (xy) plane to see if its incremental or absolute IJK's....try this (also try specifiying the G19 on a line by itself before the G3 line :
G17
G90G3X-2.0Y0.I-1.0J0.0

iF THIS WORKS THEN YOUR ijk'S ARE INCREMENTAL FROM THE START POINT. IF NOT, THEY'RE LIKELY ABSOLUTE

[slowdigits2]

In absolute i have other programs with arc in different plane and they are g90 this is a small program i use was written by the installer

G17 G20 G40 G80
G90
G54

M6 T1 (scribe)

G90
G0 X1.1 Y-0.625

G0 Z1.0

S1000 M3

G1 Z0.45 F25.
X1.
Y0.62
5
G0 Z1.
X-0.9 Y-0.625

G1 Z0.45 F25.
X-1.
Y0.625
M6 T2 (cut)


M3 S1550

G90
G0 X6.25 Y-0.75

G0 Z0.8 M08

G1 G41 X5.625 Y-0.75 D2 Z-0.875 F5.
X1.9364
G1 F12.

G3 X1.275 Y-0.5 I-0.6614 J-0.75
G1 X-1.275

G3 X-1.9364 Y-0.75 I0 J-1.

G1 X-5.875
Y0.75
X-1.9364

G3 X-1.275 Y0.5 I0.6614 J0.75

G1 X1.275
G3 X1.9364 Y0.75 I0 J1.

G1 X5.875
Y-0.75
X5.5

G0 Z10.
M9
G0
G40 X0 Y3.5

G91 G28
Z0.

G91 G28 Y0.

G90

M30

[MetalCarpenter]

I wasnt thinking correctly.the j is center of arc from where your at (incremental) .same as k.if your arcing from were the tool is at same z as center of the arc,k is 0 or just leave it out.what is the dia of the pipe and where is z0 at?

[MetalCarpenter]

Nevermind.I seen wherr you already said the od size.ill get right back to you

[MetalCarpenter]

G17 G20 G40 G80
G90 G54
M6 T3*
M3 S1550*
G0 X8. Y-3.25
G0 Z0 1. M08
G90 G0 X8. Y-3.25 Z-1.875 F5.
G1 X-8. Y-3.25 F20.
G2 G19 y3.25 J3.25 K-2.9375
G1 G17 X8. Y3.25
G3 G19 y-3.25 J--3.25 K-2.9375
G1 G17 X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
G90
M30

[MetalCarpenter]

G17 G20 G40 G80
G90 G54
M6 T3*
M3 S1550*
G0 X8. Y-3.25
G0 Z0 1. M08
G90 G0 X8. Y-3.25 Z-1.875 F5.
G1 X-8. Y-3.25 F20.
G2 G19 y3.25 J3.25 K-2.9375
G1 G17 X8. Y3.25
G3 G19 y-3.25 J--3.25 K-2.9375
G1 G17 X7.87
G0 Z10. M9
G0 G40 X0 Y3.5
G91 G28 Z0.
G91 G28 Y0.
G90
M30

The center of the radius is the center of the pipe.if the top is z0 and your at z-1.875, the center of the arc in z is -2.9375 below where your tool is so k-2.9375 should be correct.arcing from y-3.25 to y3.25, the center would be at y 0 which is 3.25 positive from where your tool is at.as far as g2 g3, when u change the plane,what it does is change the "drilling axis" so g2/g3 would be interpreted looking from the drilling axis.g19 makes the machine interpret the arcs in yz axis so x is drilling axis.looking from x positive to x0 a g2 would arc up and from y neg to y pos.a g3 should arc up from y pos to y neg.let me know if it works

[slowdigits2]

Thanks for your help again, the z 0 is in fact the top of the pipe I will try this tomorrow as soon as possible Im done work for the day again I appreciate all your help and everyone else that had comments is there a reason not to simplfy things an just use the R for the arc this is not a critical cut just plowing out a PC I have read where many have said not to use it

The center of the radius is the center of the pipe.if the top is z0 and your at z-1.875, the center of the arc in z is -2.9375 below where your tool is so k-2.9375 should be correct.arcing from y-3.25 to y3.25, the center would be at y 0 which is 3.25 positive from where your tool is at.as far as g2 g3, when u change the plane,what it does is change the "drilling axis" so g2/g3 would be interpreted looking from the drilling axis.g19 makes the machine interpret the arcs in yz axis so x is drilling axis.looking from x positive to x0 a g2 would arc up and from y neg to y pos.a g3 should arc up from y pos to y neg.let me know if it works

[MetalCarpenter]

Thanks for your help again, the z 0 is in fact the top of the pipe I will try this tomorrow as soon as possible Im done work for the day again I appreciate all your help and everyone else that had comments is there a reason not to simplfy things an just use the R for the arc this is not a critical cut just plowing out a PC I have read where many have said not to use it

Not a problem. I just prefer ijk method.It may in fact work with the r only.idk for sure.ive been told to always use ijk but that may just be as good as r.good luck

[silverslammer]

I inputted your data in my cad, this proven program you have is telling me for sure your machine wants INCREMENTAL values (from the start point) for defining the arc centre. I definintely agree with MetalCarpenter re: using IJK instead of "R"'s....if you use "R"'s the machine can sometimes go the opposite way you want to, by using IJK's this will never happen.

[slowdigits2]

Finally got around to trying it i get an error message 806 illeagl adress (rad, 0, 8) at the first g2 line
thanks again