[rajesh_1355]

Dear Friends,

I have Cincinnati VMC with Fanuc 21 m controller. while running prog for rigid tapping, quality of thread is not good.
Here under is the programme,

N1

G0G90G80G40G21
G28G91Z0.0
T1M06
G0G90G54X-23.4Y15.0
G0G90G43Z100.0H1
M03S1200
Z50.0
G83G98Z-81.0R5.0Q5.0F160.0

G0G90G80Z100.0
M05
G28G91Z0.0

and the parameter used for rigid tapping are,

N05200 P 00000001
N05201 P 00000001
N05202 P 00000001
N05203 P 00000000
N05204 P 00000000
N05210 P 29
N05211 P 200
N05212 P 0
N05213 P 1000

Cutting material is Aluminium.
Z axis motor load current is 70 %
No backlash in Z-axis.

Any suggestion , pl help.

regards.

[mactec54]

rajesh_1355

What thread size/Pitch are you cutting, Have you tried a Roll-form Tap

[angelw]

Hi Rajesh,

For starters,

G83 is a Peck Drilling Cycle.

By setting parameter 5200.0 to "1", Rigid Tapping will be invoked by G84 and not an "M" code. This is fine if you don't want to use G84 in its standard form, as Rigid Tapping will always be called when G84 is executed.

I've observed your problem with quite a few of my clients, and it appears that its associated with having the spindle started by M03 and not the Rigid Tapping cycle call up; this was confirmed by Fanuc. I would ensure the spindle is stopped via M05 when the Tapping Tool is exchanged for the previous tool, then only specify the Spindle Speed prior to executing the G84 command. However, I normally set parameter 5200.0 to "0", and parameter 5210 to either "0" or "29". Setting 5210 to "0" defaults to M29 being used to launch Rigid Tapping. I also advise using G95 (Feed/Rev), as it allows you to edit the Spindle Speed without having to remember changing the Feed Rate in the G84 block. With parameters 5200.0 and 5210 both set to "0", the program format is as follows:

Regards,

Bill

Previous Tool Ends Here
G91 G28 Z0.0 M09
G28 Y0.0 M05
M01
(M6 X 1 GUN TAP)
N2 G91 G28 Z0.0
T01 M06
G00 G90 G54 X-23.4 Y15.0
G43 Z100.0 H01 M08
G00 Z10.0
G95
M29 S1000
G98 G84 Z-20.0 R5.0 F1.0
---------
---------
---------
G80
G94
G91 G28 Z0.0 M09
G28 Y0.0 M05
M01

[rajesh_1355]

Hi Bill,
Thanks a lot for your sharing.
Definitely I m going to try this tomorrow.
Thanks A lots once again.:wave: