What is the Standard for Rigid Tapping on all Fanuc Mill Controls?????? [Archive]

View Full Version : What is the Standard for Rigid Tapping on all Fanuc Mill Controls??????

tobyaxis

03-15-2007, 11:27 PM

I was told today (in an obnoxiously rude manor, by my Supervisor) that M29 was the Standard Miscellaneous Code for Rigid Tapping in all Fanuc Mill Controls. Personally I really don't think it is true.

From my experience M-Codes vary from Mahinie Tool Builder to Machine Tool Builder.

Is M29 to be on the M-Code Standard list?

The Control is a Fanuc 0M, Machine is a Pratt & Whitney Mill Drill from around 1990-1994.

Can anyone here agree that M29 is the Standard M-Code for Rigid Tapping for all Fanuc Mill Controls?

tjones

03-16-2007, 01:23 AM

tobyaxis

03-16-2007, 03:17 AM

My fanuc 160i control has m29 for coolant valve 2.

M=machine code. The Machine builder can decide what they wish to assign the M codes to. You can also read this in the Fanuc manuals.

Fanuc does reserve certain M codes though.
M00, M01,M02,M30,M98,M99,M198

Quote from Fanuc 160i manual:
"Which M code responds to which machine function is determined by the machine tool builder."

Did you know there are up to 500 M codes available?

Just got off the Phone with a friend that worked for Fanuc for 15 Years that Confirmed this Statement.

And I Quote ""Which M code responds to which machine function is determined by the machine tool builder.""

I have no idea where this people get their information, but my Information comes from PROFESSIONAL CNC PROGRAMMERS.

That makes 3.

Thanks Tim ;).

tjones

03-16-2007, 03:49 PM

PROFESSIONAL CNC PROGRAMMERS.

:stupid::rotfl: :rotfl: :rotfl: :stupid:

WHILE[#199LE#130]DO1
#141=[#199*#131]-#604(NEXT INC POSITION)
IF[#199EQ#130]THEN#141=90.(SAFETY FOR ROUNDED NUMBERS)
#140=90.(IF #140=0 OR #141=90 THEN CHANGE CALCULATIONS)
IF[#141LT90.]THEN#140=ATAN[TAN[#100]]/[COS[ABS[#141]]](NEXT B POSITION FOR CALCULATIONS)
#142=[COS[#100]]*[#101](LENGTH IN Y FROM TOOL CENTER BEFORE C CALC)
#143=0-[ATAN[COS[#140]*TAN[ABS[#141]]]/[1.]]
IF[#141GT0]THEN#143=ATAN[COS[#140]*TAN[#141]]/[1.](TRUE C POSITION)
IF[#141EQ0]THEN#143=0
IF[#141EQ90.]THEN#143=90.-#100
#144=#170*SIN[#143](Y TO RADIUS CENTER)
#145=[[SIN[90.-ABS[#141]]]*[#101]]*[SIN[#140]](Z POSITION FOR B ROTATION)
#146=#170*COS[#143](X FOR C_LINE)
#147=90.
IF[#141LT90.]THEN#147=ASIN[SIN[ABS[#141]]*SIN[#140]]/[1.](ANGLE OF TANGENT LINE)
#148=SIN[#100]*#101
IF[#141LT90.]THEN#148=[TAN[#147]]*#145(X FOR PART ROTATION)
IF[#616EQ0]GOTO150
IF[#199GT[#130/2.]]THEN#196=0(#196+2.)
N150#149=[#751/2-#752]-[[[#755-#752]/#130]*[#199-#196]](CURRENT WHEEL RADIUS)
#150=0-[#149*SIN[#140]](Z WHEEL POSITION AT ANGLE)
#151=#149*COS[#140](X WHEEL POSITION AT ANGLE)
#152=#150+#145 (SET Z IF TRACKING WHEEL)
#153=#151 (SET X IF TRACKING WHEEL)
IF[#616EQ0.]THEN#152=#145(WHEEL CENTERED Z)
IF[#616EQ0.]THEN#153=#149(WHEEL CENTERED X)
IF[#143LT0]THEN#152=#145(WHEEL CENTERED Z)
IF[#143LT0.]THEN#153=#149(WHEEL CENTERED X)
#120=#102(FEEDRATE)
IF[#147GT50.]THEN#120=#120*1.2
IF[#147GT60.]THEN#120=#120*1.2
IF[#147GT70.]THEN#120=#120*1.3
IF[#147GT75.]THEN#120=#120*1.3
IF[#147GT80.]THEN#120=#120*1.3
IF[#147GT85.]THEN#120=#120*1.2
IF[#120GT9999.]THEN#120=9999.
IF[#616EQ0.]GOTO200
IF[#199GT1.]GOTO200
N200G55G1G90X[#153+#146+#148] Y[#142+#144-#753] Z[#152] B[#140] C#143 F#120
#199=#199+1.
END1

Like part of my macro program with 5 axis simultaneous movement?

vpcnc

03-16-2007, 08:45 PM

On All Fanuc Controls, M29 is the Default M code as supplied by Fanuc used to Activate Rigid Tapping.

However, Fanuc provides a Parameter setting so that any other Unused M code can be made to Activate Rigid Tapping.

There is also a second Parameter that can be set so that NO M code is Needed and the G84 alone will always activate rigid tapping.

The Specific Parameter Number depends on which model Fanuc Control you have.

It depends on the Machine Tool Builder, or How your Machine was Set up.
On Some Machines, M79 might be used for Rigid Tapping.
This is often true on turning Centers with Main Spindle Rigid Tapping.

Bottom Line:
Always Refer to the Instruction Manual that is supplied by the Machine Tool Builder. The Fanuc Manuals are just a general Referance.

The Machine tool Builder is the One who Really determines How your Machine / Control will work in combination.

Aside from the Parameters provided for by Fanuc, Every Function of the Machine can be controled from the PMC program. So it's possible for a Machine tool builder to use Any Code for Any function.

So to Answer you Question.
NO - M29 is not the Standard.
It is the Default if no other M code has been selected.

I was told today (in an obnoxiously rude manor, by my Supervisor) that M29 was the Standard Miscellaneous Code for Rigid Tapping in all Fanuc Mill Controls. Personally I really don't think it is true.

From my experience M-Codes vary from Mahinie Tool Builder to Machine Tool Builder.

Is M29 to be on the M-Code Standard list?

The Control is a Fanuc 0M, Machine is a Pratt & Whitney Mill Drill from around 1990-1994.

Can anyone here agree that M29 is the Standard M-Code for Rigid Tapping for all Fanuc Mill Controls?

tobyaxis

03-17-2007, 01:40 AM

On All Fanuc Controls, M29 is the Default M code as supplied by Fanuc used to Activate Rigid Tapping.

However, Fanuc provides a Parameter setting so that any other Unused M code can be made to Activate Rigid Tapping.

There is also a second Parameter that can be set so that NO M code is Needed and the G84 alone will always activate rigid tapping.

The Specific Parameter Number depends on which model Fanuc Control you have.

It depends on the Machine Tool Builder, or How your Machine was Set up.
On Some Machines, M79 might be used for Rigid Tapping.
This is often true on turning Centers with Main Spindle Rigid Tapping.

Bottom Line:
Always Refer to the Instruction Manual that is supplied by the Machine Tool Builder. The Fanuc Manuals are just a general Referance.

The Machine tool Builder is the One who Really determines How your Machine / Control will work in combination.

Aside from the Parameters provided for by Fanuc, Every Function of the Machine can be controled from the PMC program. So it's possible for a Machine tool builder to use Any Code for Any function.

So to Answer you Question.
NO - M29 is not the Standard.
It is the Default if no other M code has been selected.

Thanks for the information VPCNC however the Machine Manuals that I requested are not available. Someone that used to work there took the Manuals. So I was told.:grumble:

Tim,

Man You ROCK!!!!!!!!!!!:yourock: :banana_copy1::92:

ProfGAB

03-17-2007, 03:21 AM

M29 works on 2 machines I use.

However - I'm not sure if/when the high res spindle encoder was made standard... I work on a Kiwa Colt 510VMC that has a 0m control. Back then the high res encoder was an expensive option - Like $3000. Front office bean counters figure its not needed... even though the cost of tension compression tooling to tap using G84 ended up costing more over time. Since the machine did not come with the encoder it cannot rigidtap.

Try the following program as a test.
%
:999(RIGID TEST)
N1G0G17G40G91
G28Z0.
T1(1/4"-20 TAP)
M6

N2G0G43G54G90X0.Y0.Z2.H1
Z.5
M29S1000
G84Z-.5R.2F50.
G0Z2.
G28G91Y0.Z0.
M30
%

Do this in single block. Note the it will require several pushes of the start button before anything happens on the tap command but once it starts it will complete the cycle - and feed hold is usually disabled during the tap cycle when it executes the M29 line the spindle may twich as the spindle finds an encoder index point After M29 line, machine should move to the "R" value. (z.2) Spindle starts with sync feed to the Z value Spindle reverses with sync feed back up to "R" point Spindle stops and returns to IP (Z.5)If this works, then try taking it a step further... by adding "Q.15" to the G84 command.

It might just alarm out not recognising the M29 code.

Note that M29 defines the Sxxxx value and NO M03 is used.

(Side note Even Haas has in the programing manuals not to use an M03 for tapping - just the Sxxxx value as the machine must stop the spindle and then find the index point to begin tapping)

Machines that don't support RIGID tapping still use an M03Sxxxx with the G84 tapping cycle.

( Have I added enough smoke yet? )

tobyaxis

03-17-2007, 03:57 AM

This continues to become more interesting by the day.

This is the complete program that I have been using. Mind you this is a small machine using what seems to be 30 Taper Tool Holders. Attached is a BCC Drawing with two programs. The one on the Left is the way my Supervisor wanted it and on the Right, the way it is being done. Reason being is that these parts are 5/8 diameter 303SS collars with a 5/16 bore that is +-.0002. You get the idea behind my thinking.

%
O0103
(PRATT & WHITNEY MILL/DRILL)
(FANUC OM)
(P/N=)
(OPERATION #1)
(CAD=TEST FANUC 0M CONTROL & POST PROCESSOR)
(DATE=M-D-Y 3-15-07)
(MATERIAL=)
(XYZ)
(LWH)
(S/U=)
(CYCLE TIME=H-M-S)

G0G40G49G80G90G99M5
G91G28Z0M9
G90

N1(DOWEL PIN 1/2D)
(USE=BANK X0Y0 TWO PARTS AT 90 DEGREES)
(ON ENDS)
M6T1
G90G54G40G0X0Y0
G43Z1.0H1
Z.1
G1Z-.375F50.0
M0(LOAD PARTS)
G91G28Z0
M1

N2(C/D #3 HSS)
(USE=CENTER DRILL 4 PLACES EACH PART)
M6T2
S800M3
G90G54G40G0X-.5625Y0.56
G43Z1.0H2
Z.1M8
G99G83Z-.24R.01Q.05F2.0
Y.19
Y-.19
Y-.56
X.5625
Y-.19
Y.19
Y.56
G80M9
G90G0Z1.0M5
G91G28Z0
G49G90
M1

N3(DRILL #20 .161D 135SPT COB STB)
(USE=DRILL 4 LOCATIONS THRU EACH PART)
M6T3
S900M3
G90G54G40G0X-.5625Y0.56
G43Z1.0H3
Z.1M8
G99G83Z-.35R.1Q.025F4.0
Y.19
Y-.19
Y-.56
X.5625
Y-.19
Y.19
Y.56
G80M9
G90G0Z1.0M5
G91G28Z0
G49G90
M1

N4(TAP 10-32)
(USE=TAP 4 LOCATIONS EACH PART)
M6T4
G90G54G40G0X-.5625Y0.56S320M3
G43Z1.0H4
Z.25M8
M29S320
G99G84Z-.375R.25F10.0
Y.19
Y-.19
Y-.19
Y-.56
X.5625
Y-.19
Y.19
Y.56
G80M9
G90G0Z1.0M5
G91G28Z0
M30
%

tobyaxis

04-07-2007, 12:49 AM

This is what I have foundout about the M29 Rigid Tapping Function in Fanuc Controls.

captainasty

05-03-2007, 10:06 PM

My Hardinge VMC 1000 has 0-MD controll and it uses M29 to activate Rigid tapping.

tobyaxis

05-03-2007, 11:18 PM

My Hardinge VMC 1000 has 0-MD controll and it uses M29 to activate Rigid tapping.

It doesn't actually have Rigid Tapping if you have to Activate it. What your actually doing is telling the Machine to use the Spindle as a Servo Motor. If you actually had Rigid Tapping (a $$$$ option) you would just have to Program G74 (LH) or G84 (RH).;)

Boston

05-04-2007, 12:02 AM

Rigid Tapping
This function allows a fast and accurate tapping through
the synchronization of the spindle position loop with the tap
axis (Z-Axis).
on any newwer Fanuc controller M-29 is a defualt setting. Any machine build can reset this to whatever they want.G-84 sychronization of feed to rpm

captainasty

05-04-2007, 12:08 AM

I'm a little lost here. Your attachment states that G74 & G84 are for tapping in either rigid mode or not. My manual says that if you wish to tap in rigid mode then enter M29 before or on the same line with G74/G84. If it's not rigid tapping then how come the tap does not break when using a collet holder?:help:

Boston

05-04-2007, 12:12 AM

with M-29 the first thing that happens is the spindle will Orientate. with M-29 you can re tap a part and the thread wil not get screwwed up. With G-84 there is no spindle Orientatioin so the thread could start any postion at the same Z depth

tobyaxis

05-04-2007, 12:18 AM

Boston

05-04-2007, 12:30 AM

They both are ridge tapping M-29 spindle will Orientate. G-84 rpm and feed. In all older controller M-20 thru M-29 are customer user definded. Sence about mid 90 M-29 came on the seen

tobyaxis

05-04-2007, 01:34 AM

They both are ridge tapping M-29 spindle will Orientate. G-84 rpm and feed. In all older controller M-20 thru M-29 are customer user definded. Sence about mid 90 M-29 came on the seen

Actually 1986 or 1987 M29 was assigned Rigid Tapping. I found this in the Fanuc PDF Manual for 16, 18, 160, and 180 Controls.;)

Boston

05-04-2007, 01:43 AM

you are mostly like right I should have said that the min 90 machines I ran where the first I use M-29

tobyaxis

05-04-2007, 01:50 AM

you are mostly like right I should have said that the min 90 machines I ran where the first I use M-29

Mike I just learned about M29 2 months ago. All The CNC's that I have Programmed since 2001 never needed M29 to do Rigid Tapping LOL, just the ones I program now. We are always learning new things which means we will never get BORED LOL:p.

Cutting Tools, Machines, Controls, CAD/CAM, and PC's. We will never know everything, but we can sure keep trying;)