Contents - Index - Previous - Next

This cycle is used when NC code is created manually.

The picture shows a billet which is to be machined to leave the end at a smaller diameter.

A G0 command is used to bring the tip of the tool to starting position P0. The G84 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. Cutting movements will be at the cutting feed rate. All other movements will be at rapid traverse rate.

The best way to appreciate the cycle is to get WELturn to simulate the G84 illustration below. Copy everything between the % symbols, including the % symbols, into UNCONVERTED WINHELP MACRO:!EP(`C:\\windows\\notepad.exe',0)Notepad.Save the file in C:\WELturn\Turndata with the extension .cnc

Go into WELturn and run the file in simulation mode only: do not try to machine anything. Observe the path of the tool as it executes the cycle.

G84 illustration (metric)
%
* Billet Diameter 25
N10 T1
N20 S950
N30 G0 X25 Z5
N40 G84 X5 Z-20 F100 H2
%

Line N30 gives point P0, the point from which the G84 cycle starts.

In line N40, X5 Z-20 give P1. When the tool reaches this point it backs out by the depth of the previous cut to clean the shoulder and stops.

The full format of the G84 command is:

N(line number) G84 X(co-ord of P1) Z (co-ord of P1) F(cutting feed rate) H(depth of cut)

For example:
N150 G84 X20 Z-45 F100 H0.5

Note: the X co-ordinate is the DIAMETER at P1 and the Z co-ordinate is the distance of Z left (notice the minus sign) from the centre of the end of the BILLET, not the finished part. The centre of the end of the billet is the location of the origin, X = 0, Z = 0. All co-ordinates are ABSOLUTE values measured from this point.

From the depth of cut, WELturn calculates the number of cutting passes required. If necessary, it adjusts the depth of the final cut so that the finished diameter is correct.

It is advisable to plan G84 machining so that the part is left slightly over-size. The excess material is removed with a finishing cut at a slower feed rate.

BORING

Preparation:
Pre-drill a hole large enough for the boring tool to enter without fouling the part. Ensure that the hole is longer than the planned bored length so that the boring tool cannot run into 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 Bore Dimensions:
Diameter of pre-drilled hole 18mm
Depth of pre-drilled hole 20mm
Diameter of bore (X) 22mm
Depth of bore (Z) 15mm
Feed rate (F) 0.08mm/rev
Depth of each cut (H) 0.2mm

                    

From these dimensions, the target point, P1, for the end of the bore is at X=22, Z=-15 The starting point, P0, for boring passes is placed at X=18, Z=1 (ie at the pre-drilled hole diameter and 1mm to the right of the billet).

Note: at the end of the G84 boring cycle, the tool is left at P1, touch the far end of the bore.

The best way to appreciate the cycle is to get WELturn to simulate the G84 illustration below. Copy everything between the % symbols, including the % symbols, into UNCONVERTED WINHELP MACRO:!EP(`C:\\windows\\notepad.exe',0)Notepad.Save the file in C:\WELturn\Turndata. with the extension .cnc

Go into WELturn and run the file in simulation mode only: do not try to machine anything. Observe the path of the tool as it executes the cycle.

%
*G84 longitudinal boring example showing where the cycle ends
*Billet Diameter 30
*diameter of pre-drilled hole 18
*depth of pre-drilled hole 20
N10 T1 'select RH tool
N20 S2400
N30 G0 X30 Z60 'go to tool change position
N40 T8 'select boring tool
N50 S2400
N60 G0 X18 Z1 'position tool at starting point P0
N70 G84 X22 Z-15 F0.08 H0.2 'longitudinal boring cycle: cycle ends with tool at P1
%

Below is sample NC code for longitudinal boring which shows how the tool is brought back to the tool change position when the boring cycle is completed.

The best way to appreciate the cycle is to get WELturn to simulate the G84 illustration below. Copy everything between the % symbols, including the % symbols, into UNCONVERTED WINHELP MACRO:!EP(`C:\\windows\\notepad.exe',0)Notepad.Save the file in C:Program Files\WELsoft\\WELturn\Turndata with the extension .cnc

Go into WELturn and run the file in simulation mode only: do not try to machine anything. Observe the path of the tool as it executes the cycle.

%
*G84 longitudinal boring example