1. G42 explained?

Just to give a quick overview of me, i have been operating cnc's for about 7 yrs. at the current im in my second semester of school for programming. i have a problem that im not sure which is the correct way to program this segment of the next project. i roughed the dia. using a G02 command. im at the point that i am ready to do a finish pass im required to use a G42 command.

G42 G02 X____ Z_____ ? would this be the correct way? Or do i leave out the G02 for the following block?

2. You should lead in with a G01, then use the G42
This explains it better
http://tinyurl.com/29s9vx

Surprised that's not in any of your books?

3. i have the hand outs but it didn't explain it as such. ty for the link. ill study it a bit. thanks.

4. turn cutter comp on and feed to the start point and then make your radius.

G0X---Z--- (RAPID TO .100 OF STARTING POSITION OF RADIUS)
G42GO1X---Z----(START POSITION FOR RADIUS)
G01X---Z--- (MUST HAVE LINEAR FEED AFTER RADIUS TO TURN CC OFF)
G40 (TURN CUTTER COMP OFF)

• 450, mudracer has it correct.

If I could expand on it a bit.....

Before we call radius comp, we're programming the intersection of the horizontal and vertical tangent lines to the insert radius.

When you call radius comp the control takes over and compensates for the radius on the insert by no longer moving using the intersection of the tangent lines. It moves the insert to the intersection of the two radii.... the radius you intend to make and the radius on the insert.

Let's do a simple one. We have a 10." diameter OD. We want a .1" radius on the face of the part at the 10." dia. The part face is Z0. Let's round the 1/32" nose radius on the insert to .03" for simplicity.

N10 G0 X9.8 Z.1 [10." DIA MINUS .1 RADIUS DOUBLED]
N20 G42 G1 X9.8 Z0 F.007 [X REDUNDANCY FOR CLARITY]
N30 G3 X10. Z-.1 R.1
N40 GO X10.1 [MOVE MORE THAN DOUBLE THE INSERT RADIUS]
N50 G40 Z.1
N60 X12. Z10. [HOME].
M30 [DONE]

On the N20 line, the control will 'look ahead' to the G3 move.
It will cause the actual position to be 9.8" minus .03" x 2, or 9.74", assuming the control is working correctly.
Imagine holding a ball of .2" diameter [the .1" part radius] and a ball of .06" diameter [the .03" radius on the insert].
Hold both balls up in the air so that their centers are both aligned horizontally. Move them together so they touch. That's what you want, that's what the control does for you when you call radius comp.

On line N30, your actual Z will be Z-.13, not Z-.1. Again that's radius comp saving you from doing the math.

Notice N40. Save yourself a crash. If you rapid to only X10.01 the control will look ahead and see the Z.1 move coming and will crash down into the part. It's still in G42 [right side compensation].
Always rapid to a clearance postion more than twice the amount of the insert radius.

Have they fully explained G41 and G42?

Draw an arrow. Point it directly away from you. That's the travel direction or line of travel.
Draw a ball [representing the insert radius drawn full circle] tangent to the line of the travel on the right hand side. That's G42.
Draw a ball [again, representing the insert radius drawn full circle] on the left hand side. That's G41.

I've had a lot of new programmers try to face a part from the top down using G42. They were taught simply "G42, face and OD"
"G41, Bore" That's wrong.
See? Face a part from the top down, direction of travel.... insert on the left side with the arrow pointing away from you [turn the sketch upside down]? G41.

Back bore? Direction of travel... insert on the right side.... G42.

Back turn? Direction of travel... insert on left hand side.... G41.

See? It seems backwards from normal to them. So just think of the direction of travel, arrow pointing away from you, which side of the line the insert radius is on and it's easy.

I hope I haven't confused you.

• does anyone know if ther is a parameter to turn radius comp on. I currently can only do offsets in the x and z. I cannot enter the radius and tool. I am running a murata ms100 fanuc 18i control.

• figured 9it9 2out7.6