[mactec54]

Here is a sample of rigid tapping G-code from the Pulsar manual if you are working under Mach 3 (or without encoder feedback under other Controller software). Sorry about the lousy formatting. I couldn't figure out how make the code more readable.


(Novakon Rigid Tapping)

M6 T130 (Call the Tool Change for the ½-13 tap.)

G43 H130 Set the machine offset for the ½-13 tap.)

M08 (Turn on the coolant – DO NOT turn ON the spindle.)

G84 G98 X0.0000 Y0.0000 F150.0000 (Implement the Canned Rigid Tap Cycle, move to first hole at X = 0.0, Y = 0.0 and set the tapping Feed Rate to 150 inches per minute.)

Z0.0000 (Lower the tap to the top of the hole.)

G91 (Implement the Novakon Rigid Tapping Cycle.)

G01 (Use the specified Feed Rate to tap the hole.)

Z-1.0000 A13.0000 (Rotate the spindle clockwise 13.0000 revolutions as the tap is lowered one inch at the specified Feed Rate. If you are using BobCAD, it will automatically calculate the correct tpi.)

Z1.0000 A-13.0000 (Rotate the spindle counterclockwise 13.0000 revolutions as tap is raised one inch at the specified Feed Rate.)

G90 Z0.2000 (Implement the Absolute Distance Mode and move the tap 0.2 inches above hole.)

X1.0000 (Move to the second hole at X = 1.0 and Y = 0.0.)

Z0.0000 (Lower the tap to the top of the hole.)

[I think the sample code forgot to put a G91 here]

Z-1.0000 A13.0000 (Rotate the spindle clockwise 13.0000 revolutions as the tap is lowered one inch at the specified Feed Rate.)

Z1.0000 A-13.0000 (Rotate the spindle counterclockwise 13.0000 revolutions as tap is raised one inch at the specified Feed Rate.)

G90 Z0.2000 (Implement the Absolute Distance Mode and move to the tap 0.2 inches above hole.)

G80 (Cancel the Novakon Rigid Tapping Cycle.)

M09 M05 (Turn OFF the coolant and the spindle.)

M30 (End of program.)

%

So, does this code they used for Mach3 not work with the UCCNC software, or you are not using the original hardware. the other way you can do threading is using thread mills which is faster and more efficient the rigid tapping. and you don't need encoder feedback to do any type of thread milling, so you have other choices as well.

[Titaniumboy]

So, does this code they used for Mach3 not work with the UCCNC software, or you are not using the original hardware. the other way you can do threading is using thread mills which is faster and more efficient the rigid tapping. and you don't need encoder feedback to do any type of thread milling, so you have other choices as well.

This code does indeed work with UCCNC. I just got it working tonight. I first had to enable the A Axis. and then set Pin 7 Port 2 and Pin 8 Port 2 to the A-axis Step and Direction.

The code in practice is super simple. Just set G91, a Feed Rate, and issue a G01. Then issue a -Z and A to tap down in the CW direction. Then issue a +Z and -A to move the tap upwards in the CCW direction.

To use this rigid tapping ability means that I have to hand modify code generated by Fusion 360. I am hoping that a new encoder will let me use the Fusion 360 code without any modifications.

I plan to use thread milling in the future.

[mactec54]

This code does indeed work with UCCNC. I just got it working tonight. I first had to enable the A Axis. and then set Pin 7 Port 2 and Pin 8 Port 2 to the A-axis Step and Direction.

The code in practice is super simple. Just set G91, a Feed Rate, and issue a G01. Then issue a -Z and A to tap down in the CW direction. Then issue a +Z and -A to move the tap upwards in the CCW direction.

To use this rigid tapping ability means that I have to hand modify code generated by Fusion 360. I am hoping that a new encoder will let me use the Fusion 360 code without any modifications.

I plan to use thread milling in the future.

You could mod a Post processor for 360 to do the code output however you want it to be, so when you want to do threading you just use the modified post processor to do any Threading cycle you need, keep your regular post processor as is, if it works how you want it to for normal use.