Changing Radius To I And J Values

[macca_loto]

I use mastercam v9. I do all my toolpaths then post them to get the g code, i find it alot quicker. Thing is in the g code all my radius's are in R values and id really prefer to use the I and J method for this. How can i change this when i post it? I read a thread about it but was all double dutch to me!

CHRIS...

Similar Threads:

• Need Help!- Changing Keep values in program
• Help changing PD values in a Huanyang
• Manual Guide i Radius Values
• changing values to non modal

[anddsn]

Hello
In your post there is a line that give you the option of r or IJk . It will have a number associated with it Example(1) = r (2) =ijk
It is in the first couple of pages. Change the number to refect the format
you want. Save program out as another name.PST so if you make a mistake you still have the original.
AL

# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
sub_level : 1 #Enable automatic subprogram support
breakarcs : yes #Break arcs into quadrants?
use_rigid : 1 #Use Rigid Tapping?
arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arccheck : 1 #Check for small arcs, convert to linear
atol : .01 #Angularity tolerance for arccheck = 2
ltol : .002 #Length tolerance for arccheck = 1

[Mike Mattera]

Radius output is actually shorter code. Your machine doesn't care which format you use.

Mike Mattera

[macca_loto]

Radius output is actually shorter code. Your machine doesn't care which format you use.

Mike Mattera

We were talking about it at uni today and whilst the r or ijk values are the same thing, our teacher would prefer us to program with IJK. We lead in lead out with radius's but yeh cant use them.
Id prefer to solid the part in master cam and gen the tool path that way, much quicker for me but we have to manual program also!

CHRIS...

[ObrienDave]

To quote a manual from a Cincinnati machine:

"If the ENDPOINTS of the arc are more important, use R."
"If the curvature of the arc is more important, use IJK."

I had a problem when the R value was rounded off, using 180 degree arcs, the hole I was contouring came out of round by 8 to 10 thousanths.

Switching the post to IJK or using "break arcs into quadrants" fixed the problem.

Also when checking a contoured hole, I measure the hole at the 45 degree points.
The reason for this is, if there is a following error in your lead screws, it will show up when BOTH axes are at MAXIMUM velocity.

[Shotout]

Radius output is actually shorter code. Your machine doesn't care which format you use.

Mike Mattera

Some controllers, like the Haas, do. With IJK you can cut a complete 360 degree circle with no X,Y,Z value while R requires these values. Also with IJK the circle tolerance is +/- .0005 for the radius while with R is +/-.001 for the radius. The latter reason is probably the only really compeling one when CAM/CADing a program.

[millcat]

Your machine may not care which one you use.

BUT, if you use ijk it will care what ijk means.

Fanuc treats ijk as arc tan. Most conversationals and at least one other

control I have used - an Onsrud gantry router- treat ijk as arc center.

With Fanuc code, R = the square root of (i squared + j squared) .

With arc type switch set to arc center in your post, i(x) and j(y) are

as the name implies, the arc center, as they are in a cad system.

Some controllers have a parameter that controls how ijk is interpreted.

ijk has more plane and directional information. K represents Z in G18(xz)

and G19(yz) modes, and quadrant info by sign.

R is portable across any control I've ever run ijk isn't.

I've never heard of any difference in accuracy in modern controls though

ijk is shorter for a circular spring pass ie j-1;j-1; or helical interpolation

j-1 z-.01;j-1 z-.02;.

millcat

[ObrienDave]

It was not a problem in the control, as much as a math rounding error in MasterCam.
And, the difference from IJK to R was only .00005.

[millcat]

At 45 deg the ball screws are moving at minimum velocity.

At that moment they"re both moving at the same minimum rate.

'x' ball reaches mv at 90 and 270, 'y' 0 and 180, when the other axis

is stationary.

millcat

[Bliss]

Hello
In your post there is a line that give you the option of r or IJk . It will have a number associated with it Example(1) = r (2) =ijk
It is in the first couple of pages. Change the number to refect the format
you want. Save program out as another name.PST so if you make a mistake you still have the original.
AL

# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
sub_level : 1 #Enable automatic subprogram support
breakarcs : yes #Break arcs into quadrants?
use_rigid : 1 #Use Rigid Tapping?
arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arccheck : 1 #Check for small arcs, convert to linear
atol : .01 #Angularity tolerance for arccheck = 2
ltol : .002 #Length tolerance for arccheck = 1

Can someone help me to do this for mcx2?

thanks

[Bliss]

sorry double post

[chrisryn]

The technical term for the ijk is directional vectors. Now depending on the machine and the control the syntax for them are different. I have ran across older cnc/nc machines that won't use r so ijk is required. I have had to move that specific program from the older machine to a brand new haas mill and the control wouldn't accept the ijk as written. It was easier and quicker to go with r to get the program to run. So it all depends on the machine. I'm sure the instructor wants you to know how to use ijk if needed.

[Per_N]

Radius output is actually shorter code. Your machine doesn't care which format you use.

Mike Mattera

Not all cnc system accept the Radius "R" only. And the use of I and J instead of the "R" is faster to process for the control than the "R" command.
In high speed milling it is a big differens. But as you said, it will be more code.