Question on Rigid Tap canned cycle 4020HT CNC88HS

[MBX5]

I am using HSMworks to generate my Gcode...I need to modify the post a bit but I am having an issue with rigid tapping.... I am using a 1995 4020HT with CNC88HS control, Format 1.

Below is the post before I did some manual mods...simple chip breaking cycle on the hole drill, then into tap....

%
N1 O1234
N2 (T4 D=0.3125 CR=0. TAPER=118DEG - ZMIN=-0.75 - DRILL)
N3 (T5 D=0.375 CR=0. - ZMIN=-0.5 - RIGHT HAND TAP)
N4 G90 G94 G17 H0 E0
N5 G20
N6 G0 H0 Z0.
N8 M9
N9 T4 M6
N10 S1833 M3
N11 G4 P98
N12 E1
N13 M9
N14 X-2.5 Y-0.5
N15 H4 Z0.6
N16 G17
N17 G0 Z0.2
N18 G98 G73 X-2.5 Y-0.5 Z-0.75 R0+0.2 Q0.0781 P0.08 F9.17
N19 X-0.5
N20 G80
N21 Z0.6
N23 H0 Z0.
N25 M9
N26 M1
N27 T5 M6
N28 S150 M3
N29 M8
N30 X-2.5 Y-0.5
N31 H5 Z0.6
N32 G17
N33 G0 Z0.2
N34 G84 X-2.5 Y-0.5 Z-0.5 R0+0.2 Q0.0625
N35 X-0.5
N36 G80
N37 Z0.6
N39 M9
N40 H0 Z0.
N41 E0 X0. Y0.
N42 M30
%

Here is the post after I modified it for Fadal rigid tapping:
%
N1 O1234
N2 (T4 D=0.3125 CR=0. TAPER=118DEG - ZMIN=-0.75 - DRILL)
N3 (T5 D=0.375 CR=0. - ZMIN=-0.5 - RIGHT HAND TAP)
N4 G90 G94 G17 H0 E0
N5 G20
N6 G0 H0 Z0.
N8 M9
N9 T4 M6
N10 S1833 M3
N11 G4 P98
N12 E1
N13 M9
N14 X-2.5 Y-0.5
N15 H4 Z0.6
N16 G17
N17 G0 Z0.2
N18 G98 G73 X-2.5 Y-0.5 Z-0.75 R0+0.2 Q0.0781 P0.08 F9.17
N19 X-0.5
N20 G80
N21 Z0.6
N23 H0 Z0.
N25 M9
N26 M1
N27 T5 M6
N28 S150.1 M3
N29 M8
N30 X-2.5 Y-0.5
N31 H5 Z0.6
N32 G17
N33 G0 Z0.2
N34 G84.1 X-2.5 Y-0.5 Z-0.5 R0+0.2 Q0.0625 S150 F14.72
N35 X-0.5
N36 G80
N37 Z0.6
N39 M9
N40 H0 Z0.
N41 E0 X0. Y0.
N42 M30
%

Few weird things happening....at first it was using the F9.17 from the previous canned drill cycle....after I put the speeds in on the same line as the G84.1, it used the correct feed speed, but no matter what I do it will not use anything other than S40 on spindle speed...

Not sure what I am doing wrong?? Something with my post not putting the format correct?

Thanks for any insight.!!!

[Neal]

To make this work delete line N28 and change line N34 by deleting the "S150" and change the "F" code to 150.

Neal

[MBX5]

Thank you for that...

However - in that case what controls my Z speed if I change the F to 150 (which should be my spindle RPM)...

Thanks
Erik

[denmar]

G84.1G99FXXXX

[ad64075]

(INSERT CORRECT TOOL#, DESIRED RPM, FEED, DEPTH)
(THIS PROGRAM ASSUMES 1/2-13 TAP)


M6T3
G0 G90 E1 X0. Y0. S130 (DO NOT USE M3 IN THIS LINE!!!)
H3 Z1. M8
G84.2 (PREP FOR RIGID TAP)
G98 G84.1 X0. Y0. Z-.75 R.1 F10. S130
G0 G80 Z1. M9
M1

[MBX5]

Thanks for all the help so far.... However nothing seems to be working....for some reason the sindle defaults to S40...sometimes the feed ends up being the F9.17 from the previous operation, and there is a G80 in there to end that cycle...

Not sure whats up?

[ad64075]

Have you ever tapped on this machine before?

[Neal]

If you change the "F" code which is the RPM in Format 1, the control uses the "Q" word which is the lead of the thread to recalculate the correct feed rate.

Neal

[MBX5]

Thanks..... I figured something was up w/ the code..

Yes I have tapped with this machine, but not since switching to HSMworks...they had a default format 2, and recently setup a format 1 post....but something must still need tweaked...

[Neal]

Send me exactly what your new post spits out and I will witch hunt it for you!
xyzpro@sbcglobal.net

Neal