Contents - Index - Previous - Next

The picture shows a part with a thread.

This cycle is used when NC code is created manually.

Preparation: turn the part to the crest diameter of the thread. Plan the threaded length so that the threading tool does not hit any shoulder to the left of the threaded length. Ideally, at the end of the threaded length, cut a groove of a diameter slightly smaller than the thread root. The groove should be of sufficient width that the threading tool can stop in the middle of it without hitting any shoulder at the left of the groove. In this case, the Z length entered in the G78 command is the length of the thread plus half the width of the groove.

A G0 command brings the tip of the tool to starting position P0. This position must be slightly back from the part so that rapid returns of the tool do not score its surface. The G78 command will make the tool move in a series of rectangular paths cutting material axially until the tool tip reaches target point P1 where the cycle ends.

The X co-ordinate of P1 is the diameter of the root of the thread. So, for example, the depth of an M10 coarse thread is 0.9202mm. Therefore the diameter of the root of the thread is 10

because the only material cut is what would have been removed in the G78 cycle had the work not sprung away very slightly from the tool. In G33, the X and Z co-ordinates for each pass of the tool will be the same as in the G78 cycle.

The full format of the G33 command is:

N(line number) G X(co-ord of P1) Z (co-ord of P1) F(pitch of thread)

For example, and matching G78 above:

N200 G33 X8.1596 Z-20 F1.5

G33 only controls a pass of the tool along the thread. It will be preceded a radial G0 move from P0 to the thread root diameter. It will need to be followed by a radial G0 move away from the work. There will then be an axial G0 move back to P0. You will need to write code for these three G0 moves.

Several spring passes will be required.

INTERNAL THREADING

Preparation: drill/bore a hole equal to the crest diameter of the thread. Ensure that the hole is longer than the thread length so that the threading tool cannot run into the end of the hole. Ideally, the end of the hole should be bored to a diameter slightly greater than the thread root diameter so that, at the end of a threading cut, the tool stops in a clear area. This larger diameter should be of sufficient length that the threading tool can stop in the middle of it without hitting the end of the hole. In this case, the Z length entered in the G78 command is the length of the thread plus half the length of the larger diameter at the end of the hole.

Ensure that the tool change position is far enough from the right hand end of the billet to permit safe changing of tools, especially on a 5CNC lathe with an auto-change turret.

Example thread dimensions:
Crest diameter 18mm
Root diameter (X) 20.2mm
Length of thread (Z) 15mm
Pitch of thread (F) 1.5mm
Depth of each cut (H) 0.05mm

                    
From these dimensions, the target point, P1, for the end of the thread is at X=20.2, Z=-15 The starting point, P0, for threading passes is placed at X=18, Z=1 (ie at the crest diameter and 1mm to the right of the billet).

Note: at the end of the G78 internal threading cycle, the tool is left at P0, the position from which the cycle began.

The best way to appreciate the cycle is to get WELturn to simulate the G78 illustration below. Copy everything between the % symbols, including the % symbols, into UNCONVERTED WINHELP MACRO:!EP(`C:\\windows\\notepad.exe',0)Notepad