help with go2 go3

[vandalls]

hi all

I am a real newb at all this, basically trying to teach myself g-code by trial & error. Having problems with circles if anyone can help thanks.

I have to machine a circle that has a straight side. Thought I could do the 4/5's circle part, then just straight line machine the other side, but my cnc mill dosen't like my coding.

go x-5.0 y-16.73 (position the spindle)
g91 g03 x-5.0 y-43.27 i-24.0 j-24.0 f100. (circle code, end postion, circle center, feed rate)
g01 z-1.0 f100. (spindle lower for next run)
g91 g02 x-5.0 y-16.73 i-24.0 j24.0 f100. (circle code, end position, circle center, feed rate)
g01 z-1.5 f100. (spindle lower for next run)
... & so on.

My understanding with g02/03 is x & y are for the end postion & i & j are for circle centre?
x-5.0 y-16.73 will be the start of the circle, x-5.0 & y-43.27 will be the end of the first circle pass. BTW the circle diamter is 48.00mm.
I have added two pictures of the drawing, general & a detail.
The part will be in the vise the way it looks on the drawing. x0.0 will be from the right hand side & y0.0 will be from the top of the part.

[SCouch]

Couple things may be causing a problem. First, the G91 code is putting the control in incremental mode, when you are probably wanting it to be in absolute (G90). Second, the I & J commands are INCREMENTAL DISTANCES from the present cutter position to the arc center, no matter what mode the control is in (G90 or G91). Another thing that may cause a problem is going around the hole CCW, then going back CW. If you plan to use cutter comp I doubt it will work. I would program it CCW, then reposition the spindle and repeat the program at the next Z level.

[bshields]

Just an added note here from a guy that creates post-processors for a living for 100's of controls ove the past 25 years

the I/J circle center codes can be:

Incremental from start to center
Absolute position of the center
Incremental from center to start (YES there is at least one control that does this)...
Alternate, between incremental / absolute depending on the state of coding for the control (incremental if in incremental mode, absolute if in absolute mode).

GRANTED, the Fujitsu Fanuc method of incremental from the start to the center is probably the most commonly used, it is not the ONLY method used.

Since you don't mention the make / model of the control, there is a 99% chance that above advice will fix your problem, but then again...it might not.

Please check your programming manual to to confirm exactly what method is used to define arcs.

ALSO, some controls will not let you program any arc move that crosses a quadrant boundary, even if the arc center IS defined correctly. This means that for a 360 degree circle, you must program arc moves.

Again, these controls are by far not the most common any more, but they do exist and should be taken into account if you are just getting started in programming.

Going CW or CCW should not be an issue...a move is a move..although as mentioned, using cutter comp will preclude you performing in this manner.

Alternately, if your controller allows it, you can program using R for radius, as long as you follow the appropriate rules, which are typically:

R is positive if the arc is under 180 degrees
R is negative if the arc it 180 or over
Full 360 degree circles may typically NOT be programmed using R..so you program two arcs of 180 degrees to make a 360.

You also might want to look up the concept of MODAL commands...which means that within a certain group, it isn't necessary to REPEAT a specific G code, since it is a toggle...example: G91 makes the machine incremental. The machine STAYS incremental (G91) until a G90 is issued to make it ABSOLUTE.

Following this concept, you don't need to repeat G91 after it is issued unless you need to go back to absolute (like to find a tool change point)...

[ALLtra Mach]

Iwould start at bottom of straight and mill right on into cicrcle.make it all one motion.
Also, your x & y points must lie exactly in path. I am going to assume you got those right.
what fault are you getting?
Finally, you need to subtract 1/2 cutter dia or else add cuttter comp to your code.

[OLD_Newbie]

Send me a print and show me where x0 y0 and z0 is and I will send you gcode....

[OLD_Newbie]

G90
G70
G75
G97 S5000
G00 T1
G00 X0.663 Y0.4834 Z-1.5
M12
G00 Z-0.1
G01 Z0.25 F0.125
G03 Y-0.4834 I0. J0. F0.5
G01 Y0.4834
G00 Z-1.5
M22
G00 X0.0 Y0.0
M02

[mtlmnchr]

where is the center of the circle in x/y

[OLD_Newbie]

x0 y0
here is an example


(PGM, NAME="TEST.ANC", TYPE="A2100_274", EXEMODE="STANDARD", PATH="PATHALL", ACCESS="OPEN")
:
(MSG, NAME "TEST.ANC", CREATION DATE 29 AUG 07 - 09:34)
(MSG, OP 1 FINISH PASS TOOL 12 _250 DIA MILL)
:G90 G70 T12 M6
N10 G0 X0.663 Y0.4834 S5000 M3
N20 Z1.5 M9
N30 Z0.1
N40 G1 Z-0.25 F7
N50 G3 X-0.8205 Y0. F30 P0.8205
N60 X0.663 Y-0.4834 P0.8205
N70 G1 Y0.4834
N80 G0 Z1.5
N90 M9
N100 M5
N110 M30

[jason25]

Why not use "X Y & R" along with a cutter comp? I think it is a lot easier.

[bshields]

Please do not automagically assume that all arc centers are incremental from the arc start point.

There are other variations (not common, but there)..and since you didn't mention your control type.

These variations are:

I/J are ABSOLUTE or INCREMENTAL depending on the control state
I/J are always incremental (very common, pioneered by Fanuc)
I/J are measured not from the start to the center, but from the center to the start (not common at all, but it does exist on some controls).

Please check your control manual to be sure that you know which technique is used before you start programming.

It is also best, as mentioned if you climb mill and use cutter comp to get the best size..HOWEVER, if the tool is significantly large, you may get a comp error at the transition from the arc to the line if you try to use full radius comp.

Some controls run into this problem because of the way they 'look ahead' to determine tool motion intersection points. Sometimes in tight spaces, the 'next' point is actually 'behind' the current point..and the control alarms.

You MAY need to program for a nominal size tool, using comp only to adjust for differences once you cut a part.

[OLD_Newbie]

Many ways to do it ...just pick what ya like and make some chips...


(PGM, NAME="TEST.ANC", TYPE="A2100_274", EXEMODE="STANDARD", PATH="PATHALL", ACCESS="OPEN")
:
(MSG, NAME "TEST.ANC", CREATION DATE 29 AUG 07 - 09:40)
(MSG, OP 1 FINISH PASS TOOL 12 _250 DIA MILL)
:G90 G70 T12 M6
N10 G0 X0.663 Y0.4834 S5000 M3
N20 Z1.5 M9
N30 Z0.1
N40 G1 Z-0.25 F7
N50 G3 X-0.9455 Y0. F30 P0.9455
N60 X0.788 Y-0.5225 P0.9455
N70 G1 Y0.5225
N80 G0 Z1.5
N90 M9
N100 M5
N110 M30

[Geof]

When doing a partial circle it is often easier to use R not I, J.

Without using any numbers here is a way to write the code; Xs and Ys are the Start and Xf and Yf are the finish positions Rc the circle radius and Zu and Zd the cutter position up and down.

G90
G00 (G41 Dn) Xs Ys
G01 Zd1
G03 -Rc Xf Yf
G00 Zu
G00 Xs Ys
G01 Zd2
G03 -Rc Xf Yf
G00 Zu

This positions the cutter using tool compensation.
Moves the tool down to the cut depth
Goes around counterclockwise, the negative R tells the control to follow a path subtending greater than 180 degrees.
Lifts the tool clear.
Moves back to the start.
Moves the tool down for the second cut.
etc.
etc.

There is no direction reversal so tool comp should work fine.

Depending on how many passes you need to make it may be more compact to write it using a subroutine.