I've always used I and J (or K), except one guy at work when checking my code always *****es about the I & J (those letters seem to hurt his brain) and prefers Rs. I've usualy shyed away from them, too easy to make a mistake. Anyway I was playing at the control and G2/3 X, Y, R works (negative R works for over 18 0 deg too) cool. I was messing around with the post anyway, (new version of master cam) and put in for Rs instead of I,J,K. Went to run my first program with Rs and the control ignored the G2, ignored the R and went in a straigt line. Now this machine is running in Format 1, which I know most people despise, however it was the quickest way to get rigid tapping to work.

I was completely confused, how can a command work in MDI and not work in a program. Did I screw up? (it has happened once or twice, but as I tell myself, I make mistakes on purpose so that I can learn from them). I was a bit aggravated, since it scrapped a piece of AMS 53blahblahblah armor plate.

Any suggestions, was it the Format 1? which should have been active during MDI anyway?, or is this machine just soaking up the intelligence of the natives??

You can make a complete circle using R+ or R-...we quit using IJK's...I believe they are priamrily used when you have a glass scale and are making convolutes or splines. We use format 2 and have no problem with our R's or g2/3.......might be format 1...

IMO R style programming is for shop floor edits Only.
This method deligates to the CNC control the definition of an arc center point. If you don't know where it is, and you're at the machine control, and your calculator or PC is not at hand, then use R instead of mathematically defining the arc center by I J K.
Defining precisely by I, J and K vectors is much more accurate than using R for defining an arc move. All CNC machine controls, not just Fadal controls, make assumptions when using R style arc moves. This is why sometimes you have to fool the control by using R- (what does a negative radius look like anyway). You have to ignore the preferences of machine operators sometimes, in order to maintain accuracy and prevent headaches down the road. Radius style programming is not accurate period, on any CNC control... Save yourself a lot of trouble, go back to I, J and K arc definitions!

I agree with Scott_bob. Go back to I, J, and K definitions. It will save you alot of time and effort trying to figure out what the program is doing.

Yes I agree as well.........I must edit that we do use IJK's as well as R's...when we can..although if you know where your points are the R's can be just as effective if not in a subroutine

The "R" method can work fine, however when posting from Mastercam, I would make sure to break the arc into quadrants or you could end up with some strange results. To prove this, create a half circle of a known radius and place the circle's center at the origion. Next create arc/endpoints. Choose the endpoints of the previous arc and enter a radius .0001 larger than the first.
It is not a problem 99.99% of the time, however rounding errors do occur and during the .01%, I hope it is a cheap peice of stock.

I prefer i,j to r....

Thanx, I gave up on the R thing, a one time only experiment, and switched to Format 2. its pretty handy on the mazak conversational, but there is just too much room for errors in a business where there is just too much room for errors.

One of the conditions of the fadal is the R word must always have a sign either positive or negative.

G2 X5 Y3 R6 (wont work, will move linear)
G2 X5 Y3 R+6 (will work)
G2 X5 Y3 R-6 (will work too, opposite arc)

Little Bubba--
Your post probably out put the format for the R parameter as R1.5 for a 1.5" radius. The control MUST have the format R0+1.5 to function properly. Since there is NO radius call specified with R1.5 the machine defaulted to a G1 move.
neal