thread milling question

[panaceabea]

I am trying to run a very simple thread milling bit of code on the HAAS and I am getting a message that says unrecognized gcode when I attempt to run it . This is the same format that runs fine on my Milltronics and bridgeport and I am just curious if I need to configure the program thats generating the code slightly different to work with the HAAS controller , or if its something very simple I can just edit manualy .


%
O0630(3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G49 G40 G17 G80 G50 G90
M6 T40 (TOOL DIA. 0.5)
G20 (Inch)
M03 S3500
G64
G00 G43 H40 Z0.5
(Right hand ID Conv)
X8.05 Y-2.7125
G00 G42 P0.25 X8.3375 F30.
G00 Z0.05
G02 X8.625 Y-3.00 R0.2875
G02 X7.875 Y-3.00 R0.375 Z0.00
G02 X8.625 Y-3.00 R0.375 Z-0.05
G02 X7.875 Y-3.00 R0.375 Z-0.1
G02 X8.625 Y-3.00 R0.375 Z-0.15
G02 X7.875 Y-3.00 R0.375 Z-0.2
G02 X8.625 Y-3.00 R0.375 Z-0.25
G02 X7.875 Y-3.00 R0.375 Z-0.3
G02 X8.625 Y-3.00 R0.375 Z-0.35
G02 X7.875 Y-3.00 R0.375 Z-0.4
G02 X8.625 Y-3.00 R0.375 Z-0.45
G02 X7.875 Y-3.00 R0.375 Z-0.5
G02 X8.625 Y-3.00 R0.375 Z-0.55
G02 X7.875 Y-3.00 R0.375 Z-0.6
G02 X8.625 Y-3.00 R0.375 Z-0.65
G02 X7.875 Y-3.00 R0.375 Z-0.7
G02 X8.625 Y-3.00 R0.375 Z-0.75
G02 X7.875 Y-3.00 R0.375 Z-0.8
G02 X8.625 Y-3.00 R0.375 Z-0.85
G02 X7.875 Y-3.00 R0.375 Z-0.9
G02 X8.625 Y-3.00 R0.375 Z-0.95
G02 X7.875 Y-3.00 R0.375 Z-1.00
G02 X8.625 Y-3.00 R0.375 Z-1.05
G02 X8.3375 Y-3.00.2875 R0.2875
G00 G40 X8.25
G00 Z0.5
M5 M9
M30
%




If I should move this over to the gcode section please delete and I will post it over there but I figured since it runs fine on my other mills and not the HAAS that maybe someone in this section can easily spot what I have wrong. Thanks Rich

[Geof]

I think this is it: G00 G42 P0.25 X8.3375 F30.

On the Haas your Tool Comp command is a D number: G42 D40 in this case and you will have 0.5 entered on line 40 in the tool diameter table (if you are using diameter measure)

Incidentally you can roll all your G02's into one line by using incremental on a Haas and use I and J not R. Start off with the tool inline with the center point on the X axis and +0.375 away on the Y axis:

G91 G02 I0. J-.375 Z-.10 L11

[panaceabea]

I changed the g42 from" G42 P0.25" to "G42 D40" and made it past that line and I am now getting an error message that reads Radius in G02 or G03

[panaceabea]

Geof could I impose on you to write that as a complete simple program , I tend to pick things up rapidly from example .

[Geof]

Originally Posted by panaceabea Geof could I impose on you to write that as a complete simple program , I tend to pick things up rapidly from example .

Give me an hour or so; I have to go get Lattes for me and my two financial officers (Wife and Daughter). Some people get priority.

Incidentally I think your R error is because you are doing 180 degrees and Haas wants it as R-0.375.

Back soon.

[JWK42]

If you have Macro's enabled I have a macro to do single point threading that I can post here. I have ran this on our Simulator and the DRO's seem to be right.

%
O1243 (SINGLE POINT THREADING MACRO)
N30 (WRITTEN 03-30-2009 11:29:02)
N40 (RETURNED 03-30-2009 14:29:09)
N50 #101= 1 ( SINGLE POINT THEAD CUTTER )
N60 G17 G54 G90
N70 G40 G49 G80
N80 G53 G00 Z0.
N90 G53 G00 X-20. Y0.
( TOOL #1 IS A SINGLE POINT THEAD CUTTER )
N110 G53 G00 Z0. ( RESTART TOOL #1 HERE )
N120 G53 G00 X-20. Y0.
N130 T#101 M06
N140 S3500 M03
N150 G54 G00 G90 X0. Y0.
N160 G43 Z3. H#101 D#101 M08
( START SINGLE POINT THREAD )
N180 #124= 8.25 ( X CENTER )
N190 #125= -3 ( Y CENTER )
N200 #126= -1.05 ( Z BOTTOM OF THREAD )
N210 #118= 0.1 ( RETRACT PLANE IN Z AXIS )
N220 #107= 1 ( THREAD MAJOR DIAMETER )
N230 #120= 1 ( TOOL NUMBER )
N240 #117= 0.1 ( THREAD PITCH )
N250 #119= 0.025 ( ROUGH CUT DEPTH PER SIDE )
N260 #103= 2 ( NUMBER OF ROUGH CUTS )
N270 #121= 0.005 ( FINISH CUT DEPTH PER SIDE )
N280 #109= 30 ( CUTTING FEEDRATE )
N290 ( END OF INPUTS )
N300 #129= ABS[ #118 - #126 ]
N310 #127= #[ 2400 + #120 ] ( TOOL RADIUS )
N320 #128= #107 / 2 ( THREAD RADIUS )
N330 #131= ROUND[ #129 / #117 ] + 1 ( NUMBER OF REVOLUTIONS )
N340 #133= #103 ( COUNTER )
N350 IF [ #121 GT 0 ] GOTO370
N360 IF [ #133 EQ 1 ] GOTO500
N370 #108= [ [ #103 * #119 ] + #121 ] ( SET INITIAL PASS )
N380 G90 G00 X#124 Y#125
N390 Z#118
N400 WHILE [ #133 GT 0 ] DO1
N410 #132= [ #128 - #127 - #108 ] ( ADJUST RADIUS FOR EACH PASS )
N420 G01 Z#126 F50. ( FEED TO BOTTOM )
N430 X [ #124 + #132 ] F [ #109 * 5 ]
N440 G91 G03 X0. Y0. Z#117 I - #132 J0. F#109 L#131
N450 G90 G01 X#124 Y#125 F [ #109 * 3 ]
N460 Z#118 F75.
N470 #108= #108 - #119
N480 #133= #133 - 1
N490 END1
N500 ( START FINISH CUT HERE )
N510 #132= #128 - #127 ( ADJUST RADIUS FOR FINISH PASS )
N520 G01 Z#126 F50. ( FEED TO BOTTOM )
N530 X [ #124 + #132 ] F [ #109 * 0.5 ]
N540 G91 G03 X0. Y0. Z#117 I - #132 J0. F#109 L#131
N550 G90 G01 X#124 Y#125 F [ #109 * 3 ]
N560 Z#118 F75.
N570 G00 Z3.
N580 G53 G00 Z0. M09
(UNLOAD HERE)
N600 G53 G00 X-20. Y0.
N610 M30 (END OF MAIN PROGRAM)
%

[Geof]

I'm back!!!

Before starting I have a question: Why are you using G42? You are going around the outside using a G02 so surely it should be G41?

I copied your program and have put in extra empty lines either side of my changes.

Normallly I like to work with my work zero at the center point for the circular moves and when the work zero is someplace else I create a local (secondary) work zero using G52.

I renumbered the program and when I get back to my workshop I will run it in Graphics to make sure there are no problems.

O00000(3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G49 G40 G17 G80 G50 G90
M6 T40 (TOOL DIA. 0.5)
G20 (Inch)
M03 S3500
G64

G52 X8.25 Y-3.00 (This creates a secondary work zero at your thread centerline)

G43 H40

G00X0.0 Y1.5 Z1.0 (Move into position using the G52 work zero)

G00 G41 D40 X0.0 Y0.375 Z0.05 F30.

G91 G02 I0.0 J-.375 Z-0.1 L11 (Cut thread)
G90 G01 X0.5 Y0.375 (Move away tangentially)
G00 Z1.0 (Clear Z height)

G00 G40 X0.0 Y1.0 (Cancel tool comp)

G52 X0.0 Y0.0 (Cancel secondary work zero)

G53 G00 Z0.0 (Move Z to tool change height to get it out of the way)

M5 M9
M30
%


Here it is with all the unnecessary stuff removed and compacted up a bit.

O00000(3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G20 G49 G40 G17 G80 G50 G64 G90
M6 T40 (TOOL DIA. 0.5)
M03 S3500
G52 X8.25 Y-3.00 (Secondary work zero)
G43 H40
G00X0.0 Y1.5 Z1.0
G00 G41 D40 X0.0 Y0.375 Z0.05 F30.
G91 G02 I0.0 J-.375 Z-0.1 L11 (Cut thread)
G90 G01 X0.5 Y0.375 (Move away tangentially)
G00 Z1.0 (Clear Z height)
G00 G40 X0.0 Y1.0 (Cancel tool comp)
G52 X0.0 Y0.0 (Cancel secondary work zero)
G53 G00 Z0.0 (Move Z to tool change height to get it out of the way)
M5 M9
M30
%

[WallyL7]

Here's a quickie haas threadmill program. It will arc into the threads, and arc to finish. .150 arc lead in/out.


O0000 ( 3/4-10 THREAD )
( DIA. - .5 )
G0 G90 G40 G17 G80
T1 M6
G54 X8.25 Y-3. S12000 M3
G43 H0 Z.25
Z.1
G1 Z-1.1 F100.
Y-3.225
G3 X8.625 Y-3. Z-1.075 I.12 J.225
Z-.975 I-.375
Z-.875 I-.375
Z-.775 I-.375
Z-.675 I-.375
Z-.575 I-.375
Z-.475 I-.375
Z-.375 I-.375
Z-.275 I-.375
Z-.175 I-.375
Z-.075 I-.375
X8.25 Y-3.375 Z0. I-.375
X8.475 Y-3. Z.025 J.255
G1 X8.25
G0 Z.1
Z.25 M9
M5
G91 G28 Z0.
G28 Y0.
M30

[Geof]

Originally Posted by Geof I'm back!!! Before starting I have a question: Why are you using G42? You are going around the outside using a G02 so surely it should be G41?...

My mistake!!!

You are doing an internal thread using G02 and G42; I use G41 and G03 for internal and G41 and G02 for external and when I saw G02 my brain said "external".

Here it is for internal.

O00000(3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G20 G49 G40 G17 G80 G50 G64 G90
M6 T40 (TOOL DIA. 0.5)
M03 S3500
G52 X8.25 Y-3.00 (Secondary work zero)
G43 H40
G00X0.0 Y0.0 Z1.0
Z-1.1
G01 G41 D40 X0.0 Y-0.25 F30.
G03 I0.0 J0.3125 X0.0 Y0.375 Z-1.05
G91 G03 I0.0 J-0.375 Z0.1 L11 (Cut thread)
G00 Z1.0 (Clear Z height)
G00 G40 X0.0 Y0.0 (Cancel tool comp)
G52 X0.0 Y0.0 (Cancel secondary work zero)
G53 G00 Z0.0 (Move Z to tool change height to get it out of the way)
M5 M9
M30
%

Again I will test this on my machine.

It is similar to WallyL7's in that it arcs into the cut but it uses tool comp.

I also corrected a typo in my other post on the G41 line.

I hope I have not left any in here.

[panaceabea]

Originally Posted by JWK42 If you have Macro's enabled I have a macro to do single point threading that I can post here.

Please do , I am learning alot from this thread .

[Geof]

I was a naughty boy and did have typos/errors.

These do run but they have a different tool number. Also of course because of my misinterpretation the external thread is not the correct size for 3/4".


Incidentally if you put M05 M09 on a single line Haas will give you an error message 'Multiple Codes'.

EXTERNAL
%
O00000 (3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G49 G40 G17 G80 G50 G90
M06 T1 (TOOL DIA. 0.5)
G20 (Inch)
M03 S3500
G64
G52 X8.25 Y-3. (This creates a secondary work zero at your thread centerline)
G43 H01
G00 X0. Y1.5 Z1. (Move into position using the G52 work zero)
G00 G41 D01 X0. Y0.375 Z0.05 F30.
G91 G02 I0. J-0.375 Z-0.1 L11 (Cut thread)
G90 G01 X0.5 Y0.375 (Move away tangentially)
G00 Z1. (Clear Z height)
G00 G40 X0. Y1. (Cancel tool comp)
G52 X0. Y0. (Cancel secondary work zero)
G53 G00 Z0. (Move Z to tool change height to get it out of the way)
M05
M09
M30
%

INTERNAL
%
O00001 (3/4X10 THREAD AT X8.25 Y-3.00 1.1" depth)
G20 G49 G40 G17 G80 G50 G64 G90
M06 T1 (TOOL DIA. 0.5)
M03 S3500
G52 X8.25 Y-3. (Secondary work zero)
G43 H01
G00 X0. Y0. Z1.
Z-1.1
G01 G41 D01 X0. Y-0.25 F30.
G03 I0. J0.3125 X0. Y0.375 Z-1.05
G91 G03 I0. J-0.375 Z0.1 L11 (Cut thread)
G90 G00 Z1. (Clear Z height)
G00 G40 X0. Y0. (Cancel tool comp)
G52 X0. Y0. (Cancel secondary work zero)
G53 G00 Z0. (Move Z to tool change height to get it out of the way)
M05
M09
M30
%

Now i should get back to my fixture building.

Good job I don't have a boss to hover over me.

[panaceabea]

Geof I am getting the same error message "undefined gcode" with your file as my original one , is there something in settings I might need to turn on?