0 votes
87 views
in cnc programming by (9.0k points)

In this article, we describe how to use G70 cycle for contour finishing with G71 and G72 in CNC lathe machines with all details and examples.

G70 Cycle Introduction

Although it has a smaller G number than any of the three roughing cycles G71, G72 and G73, finishing cycle G70 is normally used after any one of these three roughing cycles. As its description suggests, it is strictly used for finishing cut of a previously defined contour.
This command is used to remove the surface of the part smoothly by removing the pass that “willingly left to the end” by the user during the processing of other cycles. This cycle processes machining in accordance with the part profile by taking chips (U2) and (W) values left for finishing turning.

The G70 command is not used alone. It is used after the G71, G72 and G73 cycles. The G70 finishing pass cycle is used if U (2) and W are valued from the G71, G72 and G73 cycles.

If 0 (Zero) is written in U (2) and W, the finish pass cycle is not written at the end of the program. With finishing pass cycle, chip removal can be done with cutters used in roughing, as well as with different cutters. The G70 command consists of a single line.

G70 Cycle Format

For this cycle, there is no difference in the programming format for various controls – it is all the same, and the cycle call is a one-block command.

The programming format for G70 cycle is:

G70 P.. Q.. F.. S..

Parameters

P = First block number of the finishing contour
Q = Last block number of the finishing contour
F = Cutting feedrate (in/rev or mm/rev)
S = Spindle speed (ft/min or m/min)


Cycle G70 accepts a previously defined finishing contour from either of the three roughing cycles, already described. This finishing contour is defined by the P and Q points of the respective cycles, and is normally repeated in the G70 cycle, although other block number references may be used – be careful here!

For safety, always use the same start point for G70 as for the roughing cycles!

Things to Know

In order to make the multiple repetitive stock removal cycles (contouring cycles) work properly and efficiently, observing the rules of their use is very important. Often a small oversight may cause a lengthy delay.

  • Always apply tool nose radius offset before the stock removal cycle is called
  • Always cancel tool nose radius offset after the stock removal cycle is completed
  • Return motion to the start point is automatic, and must not be programmed
  • The P block in G71 should not include the Z-axis value (Z or W) for cycle Type I
  • Change of direction is allowed only for Type II G71 cycle, and along one axis only (W0)
  • Stock allowance U is programmed on a diameter, and its sign shows to which side of the stock it is to be applied – sign is the X-direction relative to centerline:
    … U+ for turning – towards spindle centerline
    … U- for boring – away from spindle centerline
  • Feedrate programmed for the finishing contour (specified between P and Q points) will be ignored during roughing
  • D address in one-block format only, does not use decimal point, and must be programmed for leading zero suppression format:

D0750 or D750 is equivalent to 0.0750 depth

  • Only some control systems do allow a decimal point to be used for the D address (depth of cut) in one-block G71 and G72 cycles.

G70 Cycle Examples

G70 CNC Program Example – 1 – With G71

 Figure 35-13 – Drawing example to illustrate G71 roughing cycle – program O3505

O3505 (G71 ROUGHING CYCLE – ROUGHING ONLY)
N1 G20
N2 T0100 M41 (OD ROUGHING TOOL + GEAR)
N3 G96 S450 M03 (SPEED FOR ROUGH TURNING)
N4 G00 G41 X3.2 Z0 T0101 M08 (START FOR FACE)
N5 G01 X0.36 (END OF FACE DIA)
N6 G00 Z0.1 (CLEAR OFF FACE)
N7 G42 X3.1 (START POSITION FOR CYCLE)
N8 G71 U0.125 R0.04
N9 G71 P10 Q18 U0.06 W0.004 F0.014
N10 G00 X1.7 (P POINT = START OF CONTOUR)
N11 G01 X2.0 Z-0.05 F0.005
N12 Z-0.4 F0.01
N13 X2.25
N14 X2.5 Z-0.6
N15 Z-0.875 R0.125
N16 X2.9
N17 G01 X3.05 Z-0.95
N18 U0.2 F0.02 (Q POINT = END OF CONTOUR)
N19 G00 G40 X5.0 Z6.0 T0100
N20 M01
N36 T0500 M42 (OD FINISHING TOOL + GEAR)
N37 G96 S530 M03 (SPEED FOR FINISH TURNING)
N38 G42 X3.1 Z0.1 T0505 M08 (START POS.)
N39 G70 P10 Q18 (FINISHING CYCLE – OD)
N40 G00 G40 X5.0 Z6.0 T0500
N41 M01
N42 T0700 (ID FINISHING TOOL)
N43 G96 S475 M03 (SPEED FOR ROUGH BORING)
N44 G00 G41 X0.5 Z0.1 T0707 M08 (START POS.)
N45 G70 P26 Q33 (FINISHING CYCLE – ID)
N46 G00 G40 X5.0 Z2.0 T0700
N47 M30 (END OF PROGRAM)

Even for external finishing, the cutting tool is still programmed to start above the original stock diameter and off the front face, although all roughing motions have already been completed. A similar approach applies to the internal cut. For safety reasons, this is the recommend practice.

 There are no feedrates programmed for G70 cycle, although the cycle format does accept a feedrate. The defined block segments P to Q for roughing tool already include feedrates. These programmed feedrates will be ignored in roughing mode and will become active only for G70 cycle, during finishing. If the finish contour did not include any feedrates, then program a common feedrate for finishing all contours during the G70 cycle processing. For example, program block

N39 G70 P10 Q18 F0.007

will be a waste of time, since the 0.007 in/rev feedrate will never be used. It will be overridden by the feedrate defined between blocks N9 and N17 of program O3505. On the other hand, if there is no feedrate programmed for the finishing contour at all, then

N.. G70 P.. Q.. F0.007

will use 0.007 in/rev exclusively for the finishing tool path.

G70 CNC Program Example – 2 – With G72

The same logic described for G71 cycle, applies equally to G72 cycle.
Roughing program O3506, using G72 cycle for rough turning of the part face, can be completed by using another external tool for finishing cuts using G70 cycle:

Figure 35-15 – Drawing example to illustrate G72 roughing cycle – program O3506

O3506 (G72 ROUGHING CYCLE – ROUGHING ONLY)
N1 G20
N2 T0100 M41 (OD FACING TOOL + GEAR)
N3 G96 S450 M03 (SPEED FOR ROUGH FACING)
N4 G00 G41 X6.25 Z0.3 T0101 M08 (START POS.)
N5 G72 W0.125 R0.04
N6 G72 P7 Q13 U0.06 W0.03 F0.014
N7 G00 Z-0.875 (P-POINT = START OF CONTOUR)
N8 G01 X6.05 F0.02
N9 X5.9 Z-0.8 F0.008
N10 X2.5
N11 X1.5 Z0
N12 X0.55
N13 W0.1 F0.02 (Q-POINT = END OF CONTOUR)
N14 G00 G40 X8.0 Z3.0 T0100
N15 M01
N16 T0500 M42 (OD FACING TOOL + GEAR)
N17 G96 S500 M03 (SPEED FOR FINISH FACING)
N18 G00 G41 X6.25 Z0.3 T0505 M08 (START POS.)
N19 G70 P7 Q13 (FINISHING CYCLE)
N20 G00 G40 X8.0 Z3.0 T0500
N21 M30

G70 CNC Program Example – 3 – With G71

Finish with Same Tool

 N5 T0101;

N10 M3 S1800;
N15 G0 X83 Z0 M08;
N20 G71 U1 R1;
N25 G71 P30 Q60 U0.2 W0.1 F0.18;
N30 G1 X50;
N35 G1 Z-2;
N40 G1 X60 Z-23;
N45 G1 Z-48;
N50 G1 X76;
N55 G1 X80 Z-53;
N60 G1 Z-68;
N65 G70 P30 Q60;
N70 G00 X200 Z200 M09;
N75 G28 U0 W0;
N80 M30;

Finish with Different Tool

In such a case, we can use the example above exactly. All we need to do is to call the tool that will remove the finish pass with the offset number just above the line N65 where we write the G70 command. So in such a case, between the N60 and N75 lines of the above program would be as follows:

N60 G1 Z-68;
N62 T0303;
N65 G70 P30 Q60;
N70 G00 X200 Z200 M09;
N75 G28 U0 W0;


Need to more?

In this article, we described How to use G70 cycle for contour finishing with G71 and G72 in CNC lathe machines with all details and examples. For more details;

For your comments, suggestions and questions, you can write to us from the “Comments Section” below without registration and please consider to share this post!


Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...