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 = majo