G84 Tapping Canned Cycle
OBJECTIVES
After completing this unit, you should be able to:
- Identify and describe G84 Tapping Canned Cycle
- Locate notes for tapping speed reductions on CNC Speed and Feed chart
- Find the appropriate drill size for a hole
- Calculate the feed rate for G84
Different types of tapping processes
Form tapping
- Form taps, or forming taps, shape the material into threads. Remember, knurling is a type of forming, too.
- Form taps can be called roll taps because they roll material into the thread form rather than cutting material away.
- They are sometimes referred to as fluteless taps because they create no chips and therefore need no flutes to remove any chips.
- Form taps need to have lubricant grooves to allow lubricant along the longitudinal axis of the tap. These “lube” groves prevent a hydraulic seal which can “lock” and deform or destroy the part as the pressure builds up inside the part.
Cut tapping
- Cut taps, or cutting taps, have flutes. Flutes are necessary for two reasons.
- They provide space for removing chips out the hole’s opening. This action is also called evacuating the chips.
- Flutes allow space for coolant or lubricant to access the cutting edge.
Watch this 3:29 video: CUT TAP VS FORM TAP.
In this class, the programming is only about Cut Taps.
Cut Tapping
For any tapping operation, a hole must be drilled first. In CNC, G81 will center drill and drill before the tapping operation begins.
Tapping is a three-step process.
- Center Drill (uses G81 canned cycle)
- Drill Hole (uses G81 canned cycle)
- Tap (uses G84 canned cycle)
The code for the tapping canned cycle is G84.
G84 Variables
G99 = R plane value, initial position
F = Feed rate = RPM X Pitch [much more important or critical with tapping]
R = Position of the R plane (position above the part)
X = X-axis location of hole
Y = Y-axis location of hole
Z = Position of the Z-axis at the bottom of hole
G84 is modal. The Z position clearance location will use G98 or G99.
Tapping Speeds–the Details
There are two different points about Speed with G84 Tapping Canned Cycle.
1.) With other previous operations, we turn spindle on CW (M03). With G84 canned tapping, the M03 command will slow down operation.
In program, G84 automatically turns spindle on CW. M03 is embedded within G84 Canned Cycle. The program does not need/use M03.
2.) Look on your Tapping Speed chart from the shop class. Read notes 1 and 3.
The first note informs users that the speeds on the chart are for thru holes.
Number three is a detail to pay attention to. When there is a blind hole, the speed must be reduced by 25% to 50%.
When the Speed needs to be identified, the question that needs to be asked is, “Is this a thru hole?”
If yes, use the listed speed on the chart.
If no, find the listed speed and calculate the reduction by 25% to 50%.
Read this article about G84 Tapping Cycle from G-code Tutor. (Stop at Peck Tapping.)
Drill Size Selection Review
Call out example:
¼ – 20 UNC 2A
- ¼ = major diameter
- 20 = TPI
Equation for drill size (if I don’t have a drill chart!)
Pitch = 1/TPI
Drill size = Major diameter – pitch of threads
= .25 – 1/20
= .25 -.05
=.2
Choose drill size closest to result. e.g. .201
Tapping Canned Cycle
A couple of things need to happen.
1.) The number of TPI must match pitch and rotation
2.) At bottom of hole, spindle stops and reverses out. The reverse out of the thread hole is rapid.
G84 does all of that.
G84 uses the same variables as G81. The feedrate is different.
Program example:
| T01 M06 (#5 CD) [center drill]
G90 G54 G00 x .75 y.1.0 [1st hole location] S1000 M03 G43 H01 Z1.0 M08 |
Header for Center Drill |
| G81 G99 R.1 Z-.05 F10.0
X 2.25 [2nd hole] |
Body for Center Drill |
| G80 G00 Z1.0 M09 [cancel canned cycle]
G28 G91 Z0 M05 M01 |
Footer for Center Drill |
| T02 M06 [drill size: e.g. .201 DR] (See Review above)
G90 G54 G00 X 2.25 Y -1.0 S2500 M03 G43 H02 M08 |
Header for Drilling |
| G81 G99 R.1 Z [thickness + Radius of drill: e.g. .500 + .101 = Z -.601] F15.0
X .75 |
Body for Drilling |
| G80 G00 Z1.0 M09 [cancel canned cycle]
G28 G91 Z0 M05 M01 |
Footer for Drilling |
| T03 M06 (¼ – 20 CTap)
G90 G54 G00 X .75 Y -1.0 Is it a thru hole? Yes, run speed at 100% S1223 (from chart) [Notice no code for spindle on CW {M03}] G43 H03 Z1.0 M08 |
Header for Tapping |
Feed for Taps
Formula for Feed rate: F = RPM * pitch
- The RPM is from the CNC Speed & Feed chart
- pitch = 1/tpi
Therefore: 1223 x 1/20 = 61.15
F = 61.15
More details for Feed rate for tapping on CNC
Remember that CNC machines can be very precise with their movements. When an operator inputs the F code for the feedrate, be sure to use up to four decimals places when the calculation goes to the ten-thousandths place.
In the code example below, the calculation only went to two decimal places. The operator does not need to input 61.1500.
| G84 G99 R .1 Z .7 [See explanation below]
F 61.15 [explained above] Feed down CW to .7 Reverse up X2.25 |
Body for Tapping |
Explanation for Z .7 above
The tips or bottom of the taps have tapers. The CNC machine needs to drive the taps all the way thru onto flutes.
Use major diameter; e.g. ¼ divide by 2 = 1/8. This is the radius of the major diameter, right?
Round up to nearest 10ths place. E.g. .25/2 = .125 round up to .2 [tenths place]
Add this to thickness of part; e.g. .5 + .2 = .7 Works most of the time for the tap to cut all the way thru onto its flutes.
Therefore, Z -.7
| G80 G00 Z1.0 M09 [cancel canned cycle]
G28 G91 Z0 M05 M30 (end of program) |
Footer for Tapping |
