[bbergman]

Hi,
I have an intresting problem with the use of a 90 head attachment on the haas vf-3 mill in need of the G18 using G41 with diameter it gives me alarm not avaleble.
surely there is a way to achieve this on internal ring pocketing.
Can anyone help?

[JWK42]

Tool comp won't work in G18 or G19 depending on which axis your cutter is pointing to.
We have a macro we use to mill G12 or G13 type round pockets with a right angle head. If you have macros available I can post it here tomorrow morning. It is pointing to the Y axis or G18.

[bbergman]

Thanks ,
I do havethe standard macros and use them for tool touch of and part set home .
These pockets do have a D shape .045 deep after the top round pocket.
I will still be able to use the g18 with G12/G13 will help my program shorter
and easy to change the dia of pocket.
sounds good if this is what will happen.

[bbergman]

Will there be any cost for your help?

[JWK42]

Nope

We used the program below to mill and c-bore 3 holes on a flat bar with a right angle head
mounted on our E C-1600 Haas Horizontal. We now have a VF-3 so we don't do this part on the EC-1600 anymore. I didn't include all of the code for the whole part. I did want to show how we set our G55 system using the G10 L2 P1 & P2 method.
The two G65 subs are called with a G97 local sub call. I really like this Haas feature.
The G65 sub calls are explained in the sub. Line N160 in the hole macro looks at your tool
table to get the tool diameter for the hole macro.
The "D" shape will be another problem however.



%
O5555 (TEST 123)
N30 (WRITTEN 04-14-2007 06:09:34)
N40 (RETURNED 06-04-2009 10:14:03)
N50 (TOUCH OFF ON TOP AND OUTSIDE OF BAR)
N60 (X XERO IS TABLE CENTER)
N70 (TOOL #1 IS A .25 BALL END MILL)
N80 G10 L2 P1 X-31.898 Y-36.649 Z-25.513
N90 (TOOL # 2 IS A .5 END MILL)
N100 G10 L2 P2 X-31.898 Y-38.037 Z-25.513
(END OF INPUTS)
N110 G18 G55 G90
N120 G40 G49 G80
N130 (TOOL #02 IS A .50 END MILL)
N140 M00 ( STOP TO LOAD .5 END MILL )
N150 G53 G00 Z-20. (RESTART TOOL #02 HERE)
N160 G53 G00 Y-20.
N170 S1750 M03
N180 G18 G55 G00 G90 X14.164 Y2. Z3.1696
N190 Y0.1
N200 M97 P290
N210 G00 X0. Y0.1 Z2.
N220 M97 P290
N230 G00 X-14.164 Y0.1 Z3.1696
N240 M97 P290
N250 G00 X0. Y10.
N260 G53 G00 Z-10.
N270 (UNLOAD HERE)
N280 M30
N290 (START OF HOLE MILLING CYCLE)
N300 G01 Y0.1 F50.
N310 G65 P8981 K0.47 R0.406 F8. D80 Q0.2 U0. T2
N320 Y0.1 F50.
N330 (START OF C-BORE MILLING CYCLE)
N340 G01 Y0.1 F50.
N350 G65 P8981 K0.242 R0.5625 F8. D80 Q0.2 U0. T2
N360 Y0.1 F50.
N370 M99
%
%
O8981 (ROUND MACRO IN X/Z AXIS)
N30 (WRITTEN 05-04-2006 08:53:15)
N40 (RETURNED 08-11-2009 08:43:42)
N50 #624= #5001 ( X CENTER )
N60 #625= #5002 ( Y CENTER )
N70 #626= #5003 ( Z CENTER )
N80 #606= #6 ( K OR Z DEPTH )
N90 #618= #18 ( R OR POCKET RADIUS )
N100 #617= #17 ( Q OR DEPTH OF EACH PASS )
N110 #621= #21 ( U OR DEPTH OF FINISH PASS )
N120 #620= #20 ( T OR TOOL NUMBER )
N130 #609= #9 ( F OR CUTTING FEED RATE )
N140 #608= [ #9 * 0.666 ] (PLUNGE FEED RATE )
N150 #607= #7 ( D OR PERCENT OF CUTTER DIA )
N160 #804= #[ 2400 + #620 ] ( TOOL DIAMETER )
N170 #803= [ #804 * [ #607 / 100 ] ] ( CUT STEP OVER )
N190 #806= [ [ #625 - 0.1 ] - #606 ] ( BOTTOM OF POCKET IN Y )
N200 #827= [ [ #625 - 0.1 ] - #617 ]
N210 IF [ #827 LE #806 ] #827= #806
N220 #826= [ #618 - #804 - #621 ]
N230 #822= [ #804 + [ #803 / 2 ] - #621 ]
N240 IF [ #822 GT #806 ] #822= #826
N250 #832= #822 (SAVE 1ST #822)
N260 IF [ #822 GT #826 ] #822= #826
N270 G00 X#624 Z#626
N280 G01 Y#827 F#608
N290 G01 X [ #624 + #822 ] F#609
N300 G03 I - #822 K0
N310 IF [ #822 EQ #826 ] GOTO350
N320 #822= [ #822 + #803 ]
N330 IF [ #822 GT #826 ] #822= #826
N340 GOTO290
N350 IF [ #827 EQ #806 ] GOTO410
N360 #827= [ #827 - #617 ] (CHECK Y DEPTH)
N370 IF [ #827 LE #806 ] #827= #806
N380 G01 X#624 Z#626 F15.
N390 #822= #832
N400 GOTO280
N410 IF [ #621 EQ 0 ] GOTO450
N420 #822= [ #618 - #804 ]
N430 G01 X [ #624 + #822 ] F#609
N440 G03 I - #822 K0
N450 G03 X#624 Z#626 R [ #822 / 2 ] F20.
N460 G01 Y#625 F50.
N470 M99
%

[JWK42]

Here are some pics of the right angle head milling & c-boreing holes