CIRCLE MILL

[Scot]

Greetings to all and Happy New Year,

I have multiple holes that I need to mill to diameter. The holes are drilled to the closest nominal size and then have to be circle milled to tight tolerances. When I use the wear method for cutter comp the G41 turns on during a Z move which our machines won't read. Also the cutter comp turns off and back on between each hole. Is there any method in MasterCam software to turn cutter comp. on during a X or Y move and leave it on throughout the process? I have added my posted program below. Thanks for the help.

 

 

O0000

( JOB 03-23 DATE=07-01-04 TIME=10:23 )

( MasterCam File - )

G0 G17 G20 G40 G49 G64 G80 G90

T99

T1 ( 1-3/16 FLAT ENDMILL H-Offset 1

M6

M00 ( SET CUTTER COMP. 'D' VALUE TO ZERO )

G54 X0. Y0.

G43 H1 S1286 Z.1

M3

X1.6943 Y.0084

G1 G41 D1 Z-.125 F20.59

G3 Y.4147 I0. J.2031

Y-.3978 I0. J-.4063

Y.4147 I0. J.4063

G40 Y.0084 I0. J-.2031

G0 Z.1

M00 ( SET CUTTER COMP. 'D' VALUE TO ZERO )

G41 D1 X0. Y-2.2

G1 Z-.125

G3 Y-1.7938 I0. J.2031

Y-2.6063 I0. J-.4063

Y-1.7938 I0. J.4063

G40 Y-2.2 I0. J-.2031

G0 Z.1

M00 ( SET CUTTER COMP. 'D' VALUE TO ZERO )

G41 D1 X-1.7533 Y-.0169

G1 Z-.125

G3 Y.3894 I0. J.2031

Y-.4231 I0. J-.4063

Y.3894 I0. J.4063

G40 Y-.0169 I0. J-.2031

G0 Z.1

M00 ( SET CUTTER COMP. 'D' VALUE TO ZERO )

G41 D1 X0. Y2.3349

G1 Z-.125

G3 Y2.7411 I0. J.2031

Y1.9286 I0. J-.4063

Y2.7411 I0. J.4063

G40 Y2.3349 I0. J-.2031

G0 Z.1

T99

M06

M30

[chip]

Definitly a post adjustment. I don't think Cutter Comp can stay on (The machine would comp the position of the holes). What kind of machine are you running?

[fboike]

Try this to turn on comp.

 

pbld, n, pccdia, e

 

and pccdia should look like this.

 

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k

sccomp

if cc_pos, tloffno

 

you can turn it off at tool change.

I do form grinding in my mill so I dont want the offset turning off ether.

hope this helps

[Roger Peterson]

Even if we got past turning the cutter comp on after the Z move there is not linear move to turn it on with. If we got past that it would error out on turning cutter comp off on an arc move also. We can modify the post to turn cutter comp off after the last move... I think the real solution is to go into your circle mill operation and change your entry sweep angle from 180 to 90. This will give you a linear move that cutter comp can be turned on and off on. This should take care of it. I don't have Mastercam in front of me so entry sweep angle may not be the term used in the toolpath but you'll figure it out.

 

Let me know if that does not take care of it.

[mike_f]

if all you are doing is mill the diameters to size ( not milling the bottom of a pocket for instance) I would just use contour not circle mill. That would give you lead in / lead out functions which I don't believe you have in circle mill ( I also don't have my hasp with me tonight so I can't look at that ). You are going to feed into the wall of the circle and feed off of the wall so in my mind turning the cutter comp. on and off is a non issue. It's just another g code in your line. with lead in / out you can also override your feed rates and if there is a floor involved ramp down radially after the g41 and ramp up before the g40.

[crazy^millman]

Well if you have a big enough hole and dont tell circle mill to start in the cneter in will lead in an out also if you decrease you angle to start.

 

Crazy Millman

[Rick Damiani]

Two options:

 

- If the hole is large enough, turn on Perpendicular Entry to force a line at the start and end of the circular milling operation.

 

- If the hole is too small for that, use a contour toolpath with a smallish lead-in arc, a start point at the center of the hole, and enable the 'Plunge after first move' and 'Retract before last move' options so comp can take place outside of the hole.

[Scot]

Thank You for the replies. Using a contour toolpath ended up giving me what I needed. The "plunge after first move", and "retract before last move", as Rick suggested gave me exactly what I needed. Thanks again for the help.

 

Much Appreciated,

Scot