Threading on RW12

[lager1978]

I have a 1993 RW12 with centurion 7 control w/rigid tapping. I never did any threading on this machine and was wonderering if anyone can explain it. I tried to conversationally put a tap cycle in from the "thred" soft key. It did not work correctly. Any help would be greatly appreciated!

[panaceabea]

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.)
G20 G90
N1 G0 G40
M3 S800
G88 F[1/20] P2 R.2 ?-.75 G99
N2 G0 X0.00Y0.00
N3 G80 G1
N4 M5
M9
G32
(END OF O0102)

[panaceabea]

from the rigid tap example above here are the three important lines with a brief description of whats going on , all my rambling may be a bit more than you were asking for but hopefully will be helpful


M3 S800
(turns the spindle on at 800 rpm CW)

G88 F[1/20] P2 R.2 ?-.75 G99
(F[1/20] = RPM/20 so the spindle plunges at the correct pitch)
(P2 is a two second pause at the bottom of the hole)
(R.2 is hieght to rtract above hole )
(?-.75 is the depth to tap to )

N2 G0 X0.00Y0.00
(cooordinate of hole to tap)

N3 G80 G1
(end canned cycle)

[lager1978]

So if I want to tap a 3/8-16 the plunge feed would be RPM/16 then right. I understand everything else. Thank you so much!

[panaceabea]

thats correct 800 rpm /16 = F50 for the milltronics the g88 f eed rate for 16 tpi would be G88 f[1/16] ... , then you can change the spindle speed to what ever works best for your material/tap/coolant combination and the F[1/16] should adjust the feed rate for what ever spindle speed your running

[lager1978]

I tried it and it worked as planned...Once again Thank You!

[panaceabea]

Good deal, I love rigid tapping almost as much as thread milling. The micro 100 website has a really neat little utility to generate the gcode for thread milling for a variety of thread types

[jpawelk]

When using the rigid tap (which is an option on some machines), you do not have to calculate the rpm of the spindle. All you need to specify is the TPU and the how fast you want the spindle to rotate. The control will calculate the proper feedrate for the pitch that you specified in the conversational page.