If you have the rigid tap option push program/conversational/new then enter a program number then enter
The first screen that pops up is for program name , notes etc then push f1 to store , the next screen that pops up allows you to pick the operation , push the button for drill option
The f keys will change , so you need to push the key labled start , the page will then pop up with the drill cycle highlighted , you then push the toggle button until the cycle you want pops up , tap cycle in this case , then push the down arrow to highlight the field right below that and push the toggle key until the operation you want pops up , in this case hard right
At this point you need to push the down arrow key to highlight the features in red and enter the appropriate values , they are all pretty simple , # of threads ,spindle rpm, clearance as a positive value , and depth ,which needs to be a negative value. If your zeroed on the top of the work ( -.75 for 3/4" depth below the top of the work) . The other value on this page is pause in seconds at the bottom of the hole before reversing
Then you need to push the store button which brings you back to the drill menu page , now press the position button at the bottom and a page will pop up which allows you to enter the XY coordinates of the holes to be tapped and a z value if different from the depth value plugged in on the previous page , once you have entered the coordinate hit store to return to the drill menu page .
You can keep position to add coordinates for additional holes.
When you have everything entered that relates to the hole or holes you want to tap you just need to push the end key (f3 ithink) and it will bring you to the last page that says something like disable drill cycle and push the store button again.
Then just hit the exit button and it will save the program you have just written and your ready to go buy calling the program up from the menu and running it .
I would reccomend you generate a sample file to tap at one position and then run it by cutting air somewhere above your part a few times so you can become familiar with whats going to happen . Then maybe practice on a scrap of aluminum .
I would also save the program you wrote to a disk and open it on your computer so you can see just how simple the program is , once you figure out just how simple it is you will probably just write them manualy unless there really complex.
here is a sample of the rigid tap file written by the cent 7 controller
This file is for a 1/4x20 hole tapped at x0.00 y0.00 to a z depth of .75"
O0102 (TAP ZERO)
(Conversational File Centurion VII CNC 7.7341p C.F.)
N1 G0 G40
G88 F[1/20] P2 R.2 ?-.75 G99
N2 G0 X0.00Y0.00
N3 G80 G1
(END OF O0102)