Cutter comp on an id hole< cutter diam.??

[PaintItBlue]

gonna keep numbers very basic to keep it simple
For example if i were to mill a .500 id hole (minor) then i wanted to bring in a .375 4 point 60 degree threading cutter, to mill a thread at a major of .562. where would be the best place to apply cutter comp and how would i code it. This has got me confused becuase the book says to apply a cc move of atleast the radius of the cutter, I don;t have that much room in the hole....

our typical thread generation is like this...

major/2-tool diam/2 = g 03 thread path from bottom to top

.562/2-.375/2= x.0935(arc X end incr.) i.0468 (arc center point in X incr.)
-.0935 becomes I code for actual threading path line(arc cp in X incr., no X needed for full circle)

minor/2-tool diam/2 = g 13 path

......
......
G01 z-.500 F20.
G03 I .0468 x.0935 F3.5
G91 G03 I-.0935 Z.0625 L10
G91 G03 I-.0468 X-.0935
.....
.....

[PBMW]

This would be why I use wear comp.....

[cinomarra]

Here is how i usually do int thread mill

N5 G0 X0. Y0. (RAPID TO CENTER OF HOLE)

N10 G43 H# Z.100

N15 Z0.0

N20 G91G1 Z-.500F50. (DEPTH OF THREAD)

N25 G41 D# X.04675 Y-.04675 (.562-.375/2 =.0935/2=.04675)
(X.04675 Y-.04675 WILL PUT YOU AT 45 DEG FROM START OF THREAD)
(AND WILL ALLOW YOU TO #1 RAMP INTO THREAD,#2 TURN CUTTER COMP ON. I DON'T LIKE FEEDING IN X OR Y TO THREAD DIA, I PREFER TO RAMP INTO THREAD IN XYZ)

N30 G03 X.0935 Y0.0 Z.0078 J.04675 (45 DEG /360 DEG x PITCH = Z) (MOVEMENT : 45/360=.125 x .0625= .0078)

N35 I-.0935 Z.0625 L10

N40 X.04675 Y.04675 I-.04675 Z.0078 (RAMP OUT OR R -.04675)

N45 G40 X0 Y0

G0 G90 Z.100

WE USE A LOT OF INSERT THREAD MILLS WHICH IS WHY I LIKE TO RAMP IN AND OUT IN XYZ.THIS WORKS FOR SINGLE FLUTE THREAD MILLS ALSO

HOPE THIS HELPS

[PaintItBlue]

cinomarra, thanks for the quick reply. I follow most of what you said but i can't try it till i am at work tommorow. Was I wrong in my thinking, that you have to make a move greater than the cutter radius in your g41 block?

if so this will make life a bit easier.

N25 G41 D# X.04675 Y-.04675 (.562-.375/2 =.0935/2=.04675)
(X.04675 Y-.04675 WILL PUT YOU AT 45 DEG FROM START OF THREAD)
(AND WILL ALLOW YOU TO #1 RAMP INTO THREAD,#2 TURN CUTTER COMP ON. I DON'T LIKE FEEDING IN X OR Y TO THREAD DIA, I PREFER TO RAMP INTO THREAD IN XYZ)

In regards to ramping in, g59 z is top of work, xoyo is centerline
currently i have been doing this:

fast feed center of single point to wk thickness + 1x of lead
flat arc to 3 oclock, simple x endpoint, i=1/2 x for swing point
then if work is .500 and lead is .050 doing 12x revs (1 air 10 metal 1 air)
then a flat ramp out to x0y0

is there a better way to do thread approaches, yours seems to do a ramp in the smallest space possible, but i have to deal with blanks that vary ~ .010 in thickness


I appreciate your help, we have been getting along ok when it was only 2 cutters to match diameters, now we are trying to sync up, end mills for end threading and this 1/2 tool diameter stuff is making it harder than necessary.

[cinomarra]

the only time you have to make a move greater than your cutter radius is if you program using part geometry.what i mean is if you have a 1"square block for example.upper left is part zero. if you program the actual part dimensions,than you have to input cutter dia. or radius in offset page for that tool # ie .500",and you would also want a leadin greater than the radius.
the first reply i gave you is programmed to the centerline of the cutter.therefore your dia offset for that tool would be 0.00 in the offset page.
if you need to adjust dia of thread you would input a -.003" for ex. in the offset page if your thread was tight.this would open the effective thread dia by .003".
in response to the ramp lead in, since i use thread mills which are thread specific,it's better to lead in ramp in 3 axis. single point thread mills, flat lead in works well.you may want to slow feedrate down on your leadin.

[cadman@teluspla]

Are you using VQC on the Haas mill.
If you are the R they are looking must be greater than the radius of tool and smaller than the radius of thread major dia.
The book does not describe this operation very well.