G02 and G03 posting I and K or R

[student Erik]

In older versions of mastercam when posting G02 or G03 you just got R values. Now you get I and K. Which is better,or does it matter?

[JAMMAN]

All the same, but depends on the controller if it will understand it or not. I haven't seen anything but I/J/K in the last 15 years.

[Chris In-House Solutions]

You should be able to change the output in the control def... under arcs... radius should output R's for you and delta start center point and delta from center point should output I,j,K's but like JAMMAN said it depends on what your controller can read.

[jslaero99]

It made no differences to me up to the day when the controller made the complement of the arc instead of the desired path with 'R', since then, I,J,K all the way. From what I understood, in some specific cases, with 'R' the controller have 2 possible paths when with I,J,K it's impossible. HTH!

 

JS

[JAMMAN]

Wouldn't G17/18/19 normally determine what plane the R lies in?

[Guest CNC Apps Guy 1]

R cannot do a full circle. IJK can. R has been shown in some cases to be less precise than IJK. Most modern controls will accept both.

[mkd]

small joggle (less than cutter radius) can rarely confuse IJK where only R will work. i had a Mori blow through a wall with IJK. vericut showed good results; tell that to the part.

[JAMMAN]

I avoid that by never using comp in the controller. I will defend that method till the end, people have tried to explain it to me why I should use comp in the controller, wasted a lot of breath. The less math the controller has to do the better off I am, let mastercam do the math and post it at par.

 

I made that decision after making a mickey mouse ear pattern in what was supposed to be a rectangular pocket, I changed cutters and the cutter was like .002 bigger than the radius drawn. That was over 20 years ago and I have not trusted a controller to do math on comp since.

[gcode]

^^^^^^ +1 ^^^^^^^

 

Control comp was great in pencil cam days but it will bite you sooner or later doing complex contour work.

 

It gets even more risky when you're using a CAM system to write the code ( any CAM system).

All the software can do is guessimate what the machine will do comping off and on a contour, based on industry standards.

To make matters worse, the programmer, the CAM system and the machine have no idea what value

the operator will input for the diameter offset.

 

As far as IJK vrs R, I think IJK is the only way to go.

One of my contract customer uses R's for his lathe programs, but I never use R's for mill code..

[rsc]

It made no differences to me up to the day when the controller made the complement of the arc instead of the desired path with 'R', since then, I,J,K all the way. From what I understood, in some specific cases, with 'R' the controller have 2 possible paths when with I,J,K it's impossible. HTH!

 

JS

 

 

There are two possible paths when making an arc using R values. The controls I have worked with will always take the short path (an arc under 180 degrees) at a given unsigned R value. If you need to take the long path (greater than 180 degrees), you need to specify the R value as a negative.

 

As you can see, using an R value can lead to a bad cutter path. I prefer to use IJK because there is no question where the arc center is.

 

When I learned to write G code 35 years ago using pencilCAM (paper, pencil and calculator), there was no R programming. Everything was IJK. The first machine I programmed that used R programming was a HAAS. I used it successfully until I had to do an arc greater than 180 degrees. It followed the short path. I changed it to IJ values and it followed the correct path. Examination of the manual showed me I had to use a negative R value for greater than 180 degrees. I have not used R values since then.

 

 

Bob