Can someone please email me a sample for Hass VF-2 or somethig closer.
I will make my own post but I like to see how needs to be posted out.I am looking for mill,drill and tap with midle of program tool change.

Thanks
jozef@hwindustries.com
:rolleyes:

Here is a drilling program with tool changes for a Haas controller.

%
O102
M0 (Confirm job number: job #13264)
M0 (Confirm code: This is path #102)
M0 (Confirm action: drilling operation)
M0 (This is a concatenated toolpath)
N2 T6M6
N4 G0G43H6Z10.
N6 S1370M3
N8 G54G90
N10 G0X163.258Y344.160 (Feature: 8.8 mm drilled hole)
N12 G0Z0.M8
N14 G73G98R-47.625Z-78.800Q2.0F135.
N16 X163.258Y391.400
N18 X206.510Y266.191
N20 X247.920Y185.251
N22 X319.539Y135.965
N24 X326.770Y343.775
N26 X349.448Y201.438
N28 X338.589Y116.915
N30 X374.848Y258.588
N32 X471.552Y271.076
N34 X477.053Y170.825
N36 X490.283Y344.250
N38 X490.283Y391.400
N40 G80M5
N42 M9
N44 G28G91Z10.
N46 G28Y0
N48 G90
N50 T3M6
N52 G0G43H3Z10.
N54 S1795M3
N56 G54G90
N58 G0X44.450Y44.450 (Feature: M8 tapped hole)
N60 G0Z0.M8
N62 G73G98R-47.625Z-78.800Q2.0F180.
N64 X44.450Y539.750
N66 X69.731Y320.485
N68 X69.731Y260.485
N70 X139.731Y320.485
N72 X139.731Y260.485
N74 X590.550Y44.450
N76 X590.550Y539.750
N78 G80M5
N80 M9
N82 G28G91Z10.
N84 G28Y0.
N86 G90
N88 T8M6
N90 G0G43H8Z10.
N92 S1605M3
N94 G54G90
N96 G0X69.731Y285.485 (Feature: 8 mm reamed hole)
N98 G0Z0.M8
N100 G73G98R-47.625Z-78.800Q2.0F160.
N102 X139.731Y285.485
N104 G80M5
N106 M9
N108 G28G91Z10.
N110 G28Y0.
N112 G90
N114 T4M6
N116 G0G43H4Z10.
N118 S2160M3
N120 G54G90
N122 G0X182.308Y344.160 (Feature: 6 mm reamed hole)
N124 G0Z0.M8
N126 G83G98R-47.625Z-78.800P2.0Q2.0F165.
N128 X224.911Y271.121
N130 X229.519Y180.320
N132 X349.448Y258.588
N134 X374.848Y201.438
N136 X446.428Y179.200
N138 X471.233Y391.400
N140 X502.178Y262.702
N142 G80M5
N144 M9
N146 G28G91Z10.
N148 G28Y0.
N150 G90
N152 T4M6
N154 G0G43H4Z10.
N156 S2160M3
N158 G54G90
N160 G0X125.000Y50.000 (Feature: 6 mm tooling ball hole)
N162 G0Z0.M8
N164 G83G98R-47.625Z-78.800P2.0Q2.0F165.
N166 X350.000Y500.000
N168 X525.000Y50.000
N170 G80M5
N172 M9
N174 G28G91Z10.
N176 G28Y0.
N178 G90
N180 T2M6
N182 G0G43H2Z10.
N184 S2875M3
N186 G54G90
N188 G0X101.188Y50.000 (Feature: M5 tapped hole)
N190 G0Z0.M8
N192 G83G98R-47.625Z-78.800P2.0Q2.0F145.
N194 X148.813Y50.000
N196 X326.188Y500.000
N198 X373.813Y500.000
N200 X501.188Y50.000
N202 X548.813Y50.000
N204 G80M5
N206 M9
N208 G28G91Z10.
N210 G28Y0.
N212 G90
N214 M30
%


Dan

Thanks DAN B
looks like people do not care

Oh Boo-Hoo :D

No mill on this but there is spot, deep hole drill, peck ream (thanks Ward) and obvious tool changes.

%
O4004(BLOCK #4 .5 DRILL)
T0 M06 (.50 INCH SPOT DRILL)
G90 G80 G40 G55
S1504 M03
G43 H0
/
G00 X-1. Y-0.5 Z1.
G99 G82 R0.1 Z-0.1227 P F15.04
X-4.501
G80
G00 Z1.
M01
T2 M06 ( 1/2 DRILL FOR 14 X 1.25MM TAP)
G90 G80 G40 G55
S763 M03
G43 H2
/M08
G00 X-1. Y-0.5 Z1.
Z1.
G99 G83 R0.1 Z-2.15 Q0.05 F15.26
X-4.501
G80
G00 Z1.
M01
T3 M06 (.505 REAM)
G90 G80 G40 G55
S400 M03
G43 H3
/M08
G00 X-1. Y-0.5 Z1.
M5
M01
G84 R0.1 Z-0.75 F15.
G84 R0.1 Z-1.5 F15.
G84 R0.1 Z-2.15 F15.
G00 Z1.
X-4.501
G84 R0.1 Z-0.75 F15.
G84 R0.1 Z-1.5 F15.
G84 R0.1 Z-2.15 F15.
G00 Z1.
G80
G00 Z1.
M01
M30
%

T3 M06 (.505 REAM)
G90 G80 G40 G55
S400 M03
G43 H3
/M08
G00 X-1. Y-0.5 Z1.
M5
M01
G84 R0.1 Z-0.75 F15.
G84 R0.1 Z-1.5 F15.
G84 R0.1 Z-2.15 F15.
G00 Z1.
X-4.501
G84 R0.1 Z-0.75 F15.
G84 R0.1 Z-1.5 F15.
G84 R0.1 Z-2.15 F15.
G00 Z1.
G80
G00 Z1.
M01
M30
%

The G84 canned cycle will reverse the spindle direction when retracting the reamer. This is not a good idea; reamers should always be run in their cutting direction.

Thanks Geof,
Good information timing, I was going to do these blocks tonight.

Never thought about the reversal using the G84, only have used reamers on my manual mill.


Just looked at the toolpaths, I already had changed to a G83 but not for the reason you brought up, thanks again for spotting this error.

Ken

Tulak here is the proper post.

%
O4004(BLOCK #4 .5 DRILL)
T0 M06 (.50 INCH SPOT DRILL)
G90 G80 G40 G55
S1504 M03
G43 H0
/
G00 X-1. Y-0.5 Z1.
G99 G82 R0.1 Z-0.1227 P F15.04
X-4.501
G80
G00 Z1.
M01
T2 M06 ( 1/2 DRILL FOR 14 X 1.25MM TAP)
G90 G80 G40 G55
S763 M03
G43 H2
/M08
G00 X-1. Y-0.5 Z1.
Z1.
G99 G83 R0.1 Z-2.15 Q0.05 F15.26
X-4.501
G80
G00 Z1.
M01
T3 M06 (.505 REAM)
G90 G80 G40 G55
S400 M03
G43 H3
/M08
G00 X-1. Y-0.5 Z1.
Z1.
G99 G83 R0.1 Z-2.15 Q0.25 F15.
X-4.501
G80
G00 Z1.
M01
M30
%

Ken,

G85 is a good option for reaming as well. The feed-in and feed-out will help to eliminate fast spirals as a result of exiting at rapid.

060101-1300 EST USA

Tulak:

See a previous thread in CNCZONE that I started on a macro for tool change.

http://www.cnczone.com/forums/showthread.php?t=12545&highlight=haas+tool+change+subroutine

.

Thanks Geof,
Good information timing, I was going to do these blocks tonight.

Never thought about the reversal using the G84, only have used reamers on my manual mill.


Just looked at the toolpaths, I already had changed to a G83 but not for the reason you brought up, thanks again for spotting this error.

Ken

Tulak here is the proper post.

%
O4004(BLOCK #4 .5 DRILL)
T0 M06 (.50 INCH SPOT DRILL)
G90 G80 G40 G55
S1504 M03
G43 H0
/
G00 X-1. Y-0.5 Z1.
G99 G82 R0.1 Z-0.1227 P F15.04
X-4.501
G80
G00 Z1.
M01
T2 M06 ( 1/2 DRILL FOR 14 X 1.25MM TAP)
G90 G80 G40 G55
S763 M03
G43 H2
/M08
G00 X-1. Y-0.5 Z1.
Z1.
G99 G83 R0.1 Z-2.15 Q0.05 F15.26
X-4.501
G80
G00 Z1.
M01
T3 M06 (.505 REAM)
G90 G80 G40 G55
S400 M03
G43 H3
/M08
G00 X-1. Y-0.5 Z1.
Z1.
G99 G83 R0.1 Z-2.15 Q0.25 F15.
X-4.501
G80
G00 Z1.
M01
M30
%

Peck reaming? I don't think so. Reaming should be done straight through. A G81 feeds to depth and rapids out. A G85 feeds in and feeds out.

A G82 feeds in and dwells at depth then rapids out. (I don't see any advatage of dwelling in reaming a hole.)

Drilling should be done with G81, unless the hole depth of the hole is 4 or more times the diameter of the drill. G83 peck drills and pulls the drill out with chips, rapids to the last depth and drills to the next depth until final depth.

G73 is chip breaking routine, pecks but does not pull the drill out to clearance plain. This is to break up the chips. (Like you would get drilling plastics.)

A G82 is for counter sinking where you want to control the depth to better control the diameter of the c'sink. For example, 100 deg c'sink, .002 depth is .005 on the diameter. A G82 can be used for drilling if you must control the drill depth to a close dim. The dwell probably should not be more than 3 revolutions. At least 1 revolution. If the dwell is in milliseconds then the P word value would be equal to the integer value of 60000 divided by the RPM for 1 revolution. An example of 2 revolutions at 1504 RPM, P80 ( 79.787 = 2 x 60000 / 1504)

Anyway, peck reaming makes no sense. Your hole size for reaming should be about 2% times the square root of the reamer dia smaller than the reamer dia. For example .505 reamer you would want a hole size of close to .491 dia (.4907 = .505 - .02 x sqr(.505)) You would not want to use a drill no smaller than 31/64 or .484 dia. A 12.5MM (.492 dia) drill would be ideal. If you use 1/2 drill for .505 reamer, that will work. But you are leaving less than .0025 per side for reaming. For that little material, peck reaming is . . . out of the question. If you are leaving so much material that you think you need to do peck reaming, you are leaving too much material. The bottom line, peck reaming should never be done.

Paul,
If you look again you will see that there was no G82 used in the Reaming it was used in the Spot operation, no dwell was used, since P had no value I am assuming it is ignored.

My thinking on the pecking was simply mimicking how I did manual reaming so it seemed appropriate at the time.

In retrospect, pecking would seem to offer no benefit, however, it did not seem to cost anything but some extra time, since they turned out very well.

Thanks for the formula for the hole size and advice, it is noted.

Ken