[MetalMolder]

Need to program 5/16-18 tap in format 2 could someone show me the proper way to construct the line.
Thankyou in advance

[Neal]

G84.1 G99 R0+.200 F20. S1000 Z-.5 X_____ Y ______

This format will work for Format 2 only. Format 1 programs differently.
Here's full program sample:
%
N1O432(Rigid TAPPING IN FORMAT 2
N2M6T1(8-32 TAP
N3G0G90G80G17G40S1500M5E1X0Y0 (-------------notice M5 instead of M3
N4H1Z0.2M8
N5 G84.1 G99 R0+.2 Z-.5 S1500. F46.875 X1. Y-2
N6X2.
N7X3.
N8G80M5M9
N9G0Z1.
N10X0Y0Z0H0E0
N11M2
%

[DareBee]

Neal it's pretty hard to argue with you considering your position but....

What about the G84.2 (prepare for rigid tap)?

The manual also does not show the use of an M5 as you have, is this something that you like to use for double redundancy?
I have never used it for rigid tapping.

[dpark1]

Here is all you need for the tap to work correctly:


N1 O0832 ( 8-32 tap )
N2 ( CREATED ON 04-21-08 AT 10:16 PM )
N3G20
N4G0G17G40G80G90
N5 ( #8-32 TAPRH TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA - .164 )
N6T1M6
N7G0G90S160.1M5M90E1X0.Y0.
N8H1Z1.M8
N9G84.2
N10G84.1G98X0.Y0.Z-.5R0.1S160.1F5.
N11G80
N12M5M9
N13G90H0Z0.
N14E0X0Y0
N15M30

[DareBee]

dp's program looks good to me, except for....
As mentioned I have never used the M5.
Also Fadal recommends a minimum clearance (R value) of .4, I don't know if this has to do with drive syncing or what?

Neal will hopefully supply additional comments/explanations today.

[Neal]

Darebee--
The older machine required the G84.2 to calibrate the Z axis and the Spindle motor and sync them together. HOWEVER, starting with late 1996 software the calibration cycle was included inside the G84.1 code. Therefore using the G84.2 would now run the calibration twice. A waste of time. After the introduction of the SUYSTEM 97 software the G84.2 actually became a detriment causing a "SPINDLE WOULD NOT STOP" error under certain circumstances.
Since it is not needed why use it?

Neal

[DareBee]

Thanks Neal
That explains that, my machine is a 94 and it is required.
What about the M5?

[Neal]

The M5 code is recommended as a safety precaution. If the spindle is running when the calibration takes place there is a potential for a mis-calibration to occur. Having the M5 in the program ensures that the spindle is stopped first.

Neal

[DareBee]

Perfect explanation thank you.

[perrettamachine]

N585T1M6
N586* OPERATION 14: HOLES
N587* 10MM
N588* TOOL 1: .394 TAP
N589* CS#2 - YZ PLANE
N590* E2 = X0. Y0. Z0.
N591* HEAD ON RIGHT SIDE
N592S500.2
N593G84.2
N594G19G90G0Y3.344X.5E2
N595Z-.817H1
N595.1M7
N596G8
N597M3
N598G1X-.75
N599X.5M4
N600G0M5
N601X1.
N602G0G90M5M9
N603G53Z0
N604G90G0X0.Y0.
N605Y0Z0E0H0
N606M30