G73 Pattern Repeating Rough Turning Cycle: Working Principle, Parameters, Control Differences and Alarm Solutions

G73 is a pattern-repeating cycle that, on FANUC-controlled CNC lathes, removes roughing stock by repeating the defined finished part profile a set number of times. In FANUC manuals it appears under names such as Pattern Repeating, Pattern Repeating Cycle, or Profile Repeating Cycle. The basic purpose of G73 is, when the raw material already has a shape close to the finished part, to repeat the same profile path each time shifted slightly in X and Z.

G73 is therefore suitable for cast parts, forged parts, pre-roughed parts, near-net material out of a mould, parts whose raw shape resembles the finished profile, and complex contours that change in both X and Z. FANUC sources clearly state that G73 is designed to efficiently machine parts whose rough shape has been pre-formed by casting, forging or pre-machining.

📷 IMAGE AREA — G73 pattern repeating: raw cast/forged shape, finished profile and shifted parallel passes
Suggested alt text: G73 pattern repeating rough turning diagram

1. The basic difference of G73 from G71 and G72

G71, G72 and G73 are in the same multiple repetitive cycle family, but their stock-removal methods differ. G71 mostly divides into layers in X and cuts along Z in each layer (lengthwise roughing). G72 divides the material into layers in Z and makes a facing cut along X in each layer. G73 does not cut individual horizontal or vertical strips; it runs the whole profile written between P and Q at the first roughing position, reduces the X and Z shifts and runs the same profile again, continuing until the set number of repeats is complete; on the last pass it approaches the finishing allowance and at the end of the cycle returns to the start point.

2. Very important correction: there is no Type I and Type II in G73

The Type I / Type II selection in G71 and G72, the choice based on one or two axes in the first P block, and the monotonic-profile / pocket distinction do not apply to G73. Because G73 already repeats the whole profile between P and Q, a profile containing both X and Z moves can be used; the profile does not have to be monotonic in one direction like G71 Type I; there is no requirement to write W0 or U0 to select Type II, and the number of axes in the P block does not turn G73 into Type I/II. Therefore “G73 Type I” or “G73 Type II” headings are technically incorrect. In the old and new FANUC alarm lists the monotonicity alarm is defined only for G71 and G72; there is no such Type I/II monotonicity alarm for G73. Even so, the G73 profile must be a safe, cuttable geometry that the tool can follow without collision on each repeat.

3. On which parts should G73 be used?

G73 is very efficient when the outer shape of the raw part is close to the finished profile. Suitable examples: forged crank-like profiles, cast pulleys, flanges out of a mould, pre-turned shafts, conical and stepped forged parts, and parts with roughly equal wall thickness along the profile. Unsuitable examples: removing a large amount of stock from a solid round bar, a very wide and irregular gap between the raw diameter and the finished profile, an unknown raw shape, and different, uncontrolled stock thickness at each point. If a standard stepped shaft is to be machined from a solid bar, G71 is usually more suitable; G73 should be preferred when the raw shape resembles the finished shape.

4. The classic two-line G73 format

G73 U(Δi) W(Δk) R(d);
G73 P(ns) Q(nf) U(Δu) W(Δw) F(f) S(s) T(t);

Example:
G73 U14.0 W14.0 R3;
G73 P100 Q180 U0.4 W0.2 F0.25;

The FANUC 21i, Series 0/00/0-Mate and Series 0-TD manuals show the same basic two-line structure.

5. Meanings of the G73 addresses

In G73 too there are two different U and two different W values: the first-line U and W set how far the profile is shifted in X and Z from the first roughing pass to the last, while the second-line U and W are the X and Z finishing allowances. The meaning of U and W changes according to whether P and Q are present in the same G73 block; FANUC manuals note this specifically.

6. U on the first line: total shift in X

In G73 U12.0 W6.0 R4; the U12.0 sets how far in total the profile starts from the outside or inside in X (in FANUC manuals, Δi). Important difference: the first-line U of G73 is not a single-pass depth of cut as in G71; it is the total X distribution between the first roughing profile and the last. The control divides this total by the repeat count given by R and, on each repeat, brings the profile step by step closer to the finished shape.

6.1 Whether the U value is diameter or radius

FANUC manuals define Δi as the shift amount in the X-axis direction and state that this value is given as a radius value. For example, if G73 U12.0 ... is interpreted as radial 12 mm, the difference on the diameter can be 24 mm. However, the control generation, program format, X-axis diameter/radius setting and the machine builder compatibility settings must be verified before use. In FANUC examples the X shift on the first G73 line is explained as a radius value even though diameter programming is used.

7. W on the first line: total shift in Z

In G73 U12.0 W6.0 R4; the W6.0 is the total shift of the profile repeats in Z (in FANUC manuals, Δk). This value is not a depth of cut, a finishing allowance, or the Z move on each repeat; it is the total Z shift between the first and last roughing profile. The control distributes this value according to the repeat count and, on each pass, brings the profile closer to the finished contour.

8. R on the first line: repeat or division count

In G73 U12.0 W6.0 R4; the R4 states that the profile is repeated in four divisions. In G73, R is not the retract amount of G71/G72, not a distance, and not a depth of cut; it is the profile repeat/division count. This difference is critical: G71/G72 first-line R → retract distance; G73 first-line R → repeat/division count.

9. How is the real pass amount calculated in G73?

G73 distributes the total X and Z shift according to the R count. With a simplified teaching approach: X step ≈ Δi / repeat count, Z step ≈ Δk / repeat count. For example, for G73 U12.0 W6.0 R4; the X step ≈ 12/4 = 3 mm radial and the Z step ≈ 6/4 = 1.5 mm; each new profile approaches the finished contour by ~3 mm in X and ~1.5 mm in Z. However, the real tool path can differ by control generation because of how the first and last passes are counted; in particular there is an important difference between 0i-C and 0i-D in how the R1 command is interpreted.

10. MAJOR CONTROL DIFFERENCE: R1 behaviour

There is an important difference between FANUC 0i-C and 0i-D in interpreting the G73 division count. 0i-C: even if R1 is written, the division count is applied as 2; for R2 and larger the written value is used. 0i-D: the division count written with R is applied directly, and R1 is treated as one division. The 0i-C comparison table in the 0i-D manual shows this difference clearly. Result: the same G73 U10.0 W4.0 R1; program may not produce the same number of tool paths on 0i-C and 0i-D; when a G73 program is copied from another machine, the control generation must be verified.

11. P and Q: the boundaries of the finished profile

In G73 P100 Q180 ...; P100 indicates the profile starts at line N100 and Q180 that it ends at N180. Example:

N100 G00 X50.0 Z0.0;
N110 G01 Z-20.0;
N120 X70.0 Z-35.0;
N130 Z-55.0;
N140 G02 X90.0 Z-65.0 R10.0;
N150 G01 X110.0 Z-80.0;
N180 Z-100.0;

G73 repeats this whole profile with different X-Z shifts.

12. The first profile block of G73

The first profile block marked by P must contain G00 or G01. Correct: N100 G00 X50.0 Z0.0; or N100 G01 X50.0 Z0.0;. Wrong: N100 X50.0 Z0.0;. Even if a previous modal G00/G01 is active in some cases, FANUC requires this command to be explicitly present in the first cycle block. If there is no G00 or G01 in the first P block, P/S065 can occur on old controls and the corresponding profile alarm on new 0i-D systems.

13. Profile freedom in G73

One of the important advantages of G73 is that it does not require profile monotonicity like G71 Type I. The profile can contain diameter increase, diameter decrease, different slopes in Z, tapers, convex/concave radii, steps and reversing contours. However, “the profile is free” does not mean the tool can machine every shape without collision, that undercuts are automatically safe, or that the stock thickness will be equal on every pass. The person preparing the profile must check that the tool can enter the profile on each pass, does not hit the part on the return, that the insert geometry is suitable for the undercut, and that there really is enough and balanced allowance in the raw stock.

14. U on the second line: X finishing allowance

In G73 P100 Q180 U0.4 W0.2 F0.25; the U0.4 is the finishing allowance in X. This value is not the total X shift on the first line or the roughing pass amount; it is the X allowance to be removed with G70 or a separate finishing operation. On diameter-programmed systems U is usually interpreted in diameter-value logic, but the control and program format must be verified. On an outside diameter a positive U usually leaves material outside; on an inside diameter the sign direction can be reversed.

15. W on the second line: Z finishing allowance

In G73 P100 Q180 U0.4 W0.2 F0.25; the W0.2 is the finishing allowance left in Z, and must be chosen positive or negative according to the profile direction. A wrong W sign can spoil the shoulder dimension, drive the roughing pass into the finish profile, leave no material in some regions during G70, or leave excess allowance on the face.

16. U and W signs in G73

FANUC manuals state that there are four basic cutting patterns for G73 and that the signs of Δi, Δk, Δu and Δw must be watched; that is, the first- and second-line U and W can be positive or negative, and when the cycle finishes the tool returns to start point A. The signs should not be memorised; draw the finished profile, determine which side the raw profile is on relative to the finished profile, find the X and Z shift directions of the first roughing profile, determine on which side of the finished surface the finishing allowances should remain, and verify with graphics/simulation.

17. The behaviour of F, S and T within G73

The F, S and T values given in the G73 call block or before the cycle are used in the roughing profile repeats. The F, S and T commands written between the P–Q profile blocks are ignored during G73 roughing. For example, while running G73 P100 Q180 U0.4 W0.2 F0.28 S180;, even if there is an N110 G01 Z-20.0 F0.12 S220; inside the profile, F0.28 and S180 are used in the roughing passes; the F and S values in the profile blocks can be effective only in the G70 finishing cycle.

18. The relationship between G73 and G70

After G73 removes the roughing stock, the same P–Q profile can be finished with G70. G70 cleans the X and Z finishing allowances left by G73 and machines the final dimension of the profile; when complete the tool returns to the start point and the next block is read.

19. FANUC source example

N010 G50 X260.0 Z220.0;
N011 G00 X220.0 Z160.0;
N012 G73 U14.0 W14.0 R3;
N013 G73 P014 Q019 U4.0 W2.0 F0.3 S0180;
N014 G00 X80.0 W-40.0;
N015 G01 W-20.0 F0.15 S0600;
N016 X120.0 W-10.0;
N017 W-20.0 S0400;
N018 G02 X160.0 W-20.0 R20.0;
N019 G01 X180.0 W-10.0 S0280;
N020 G70 P014 Q019;

In this example the total X shift is 14 mm, the total Z shift 14 mm, the repeat/division count 3, the X finishing allowance 4 mm, the Z finishing allowance 2 mm, the roughing feed 0.3 mm/rev, the roughing S value 180 and the finishing feed inside the profile 0.15 mm/rev.

20. Training G73 outside-profile example

%
O7301
(G73 PATTERN REPEATING ROUGH TURNING)
G21
G18
G40
G99
G50 S2200
T0101
G96 S170 M03
M08
G00 X126.0 Z4.0
G73 U8.0 W4.0 R4
G73 P100 Q180 U0.4 W0.2 F0.25
N100 G00 X52.0 Z0.0
N110 G01 Z-18.0 F0.12
N120 X64.0 Z-28.0
N130 Z-45.0
N140 G02 X84.0 Z-55.0 R10.0
N150 G01 X96.0 Z-70.0
N160 Z-88.0
N170 X108.0 Z-98.0
N180 Z-110.0
G00 X150.0 Z50.0
T0202
G96 S210
G00 X126.0 Z4.0
G70 P100 Q180
G00 X180.0 Z120.0
M09
M05
M30
%

21. Explanation of the example program

• G00 X126.0 Z4.0 the tool comes to the G73 start point A; this point must be outside all shifted profiles and collision-free on the return.
• G73 U8.0 W4.0 R4 total X shift 8 mm (radial), total Z shift 4 mm, repeat/division count 4.
• G73 P100 Q180 U0.4 W0.2 F0.25 profile N100–N180, X allowance 0.4, Z allowance 0.2, roughing feed 0.25 mm/rev.
• N100 G00 X52.0 Z0.0 the first profile block marked by P — G00 is written explicitly.
• G70 P100 Q180 cleans the finishing allowance left by G73 over the same profile.

📷 IMAGE AREA — In G73 the total X/Z shift is divided by the R repeat count so the profile approaches the finished contour step by step
Suggested alt text: G73 profile shift and repeat count distribution

22. How to choose the G73 start point

The G73 start point must be chosen more carefully than in other roughing cycles, because the whole profile will be repeated at different X-Z positions. The start point must be outside the first shifted roughing profile, away from the raw part, where the tool holder will not collide, and in a position that provides enough room for all X/Z shifts. If the start point is too close, the first shifted profile may plunge into the raw material in rapid, the tool may hit the part on return, and more stock than expected may form on the first pass. If it is too far, the cycle time grows, unnecessary idle motion occurs on each repeat, and if constant surface speed is used the speed transitions can increase.

23. The importance of the raw stock shape in G73

The G73 program knows only the finished profile and the shift amounts; the control does not directly measure the real dimension of the raw part. The programmer assumes the raw profile is a shape similar to the finished profile shifted in X and Z. If the real raw part does not match this assumption, the tool cuts air in some regions, enters excessive stock in others, cuts directly at full depth on the first pass at some points, and the pass distribution is not equal. Therefore, before using G73, the minimum/maximum diameter, length dimensions, casting tolerance, axis runout and clamping position of the raw part should be measured.

24. How to choose the total shift in G73

The first-line U and W values must cover the approximate total difference between the raw part and the finished profile. Total X shift: find the largest radial allowance in X — e.g. raw Ø120, finished max Ø100, diameter difference 20 mm, radial difference 10 mm → theoretical U10.0; but a safe value is chosen by adding the finishing allowance, casting tolerance, surface defect and clamping runout. Total Z shift: find the largest difference in Z between the raw and finished profile — e.g. raw shoulder Z-42, finished shoulder Z-48, difference 6 mm → theoretical W6.0.

25. How to choose the R repeat count

When determining the repeat count, the total X and Z shift, the insert capacity, material type, part rigidity, spindle power, chip breaker and casting skin must be evaluated together. If R is too small, the stock thickness between repeats increases, the insert can be overloaded, the depth can be very high in some regions, and vibration/tool breakage can occur. If R is too large, the cycle time grows, the tool follows the same profile unnecessarily, idle cutting increases and rubbing/edge wear can increase on the cast surface.

26. Parameters related to G73

The main G73 parameters have different numbers by control generation.

27. Old Series 0/00/0-Mate G73 parameters

The manual states these values are modal, retained until a new value is given in the program, and that a command given from the program can change the corresponding parameter value. That is, on old controls the values of G73 U14.0 W8.0 R4; not only apply to the current cycle but can also affect the modal settings; therefore the first G73 line must not be omitted in the next program.

28. FANUC 0i-C G73 parameters

On the 0i-C, 5135 and 5136 are two-word numeric parameters; the value range covers positive and negative directions. 5137 is in cycle-count units and its valid range starts from 1.

29. FANUC 0i-D G73 parameters

For turning, the axis order in the G18 plane must be evaluated according to the manual notation; the X and Z counterparts must be verified with the screen/manual version. The 0i-D manual states that 5136 is a real-number path parameter, can take a positive or negative value, must be entered as a radius value, and is not used in the Series 10/11 program format.

30. Why should you not trust just the number for 5135 and 5136?

While the 0i-C manual explains 5135/5136 directly as the X and Z directions, the 0i-D manual may define them via the first and second axes of the plane. In addition, the axis order in the G18 plane, the machine axis configuration and the Series 10/11 compatibility format can affect interpretation. Therefore, if 5135 or 5136 is to be changed, the full name of the control model must be determined, its own parameter manual opened, the axis definition read, the current value backed up, and a small safe test performed.

31. Parameter 5102 RFC and G73

On the FANUC 0i-C, 5102#4 RFC determines whether tool-nose radius compensation is applied on the G73 cutting pattern. If RFC=0 it is not applied; if RFC=1 partial compensation is applied. According to the 0i-C / 0i-D comparison, partial compensation can be selected with RFC during G71–G73 on the 0i-C, while on the 0i-D the RFC bit does not exist and tool-nose radius compensation is applied during G70–G73.

32. Tool-nose radius compensation on old controls

The old Series 0/00/0-Mate manual states that normal tool-nose radius compensation is disabled during the G73 cycle. However, a special behaviour is described whereby, if the imaginary tool-nose number is 0 or 9, the compensation value can be added to U and W; this is not the same as modern 0i-D behaviour. Therefore it is not correct to treat an old Series 0 program, a 0i-C program and a 0i-D program as the same in terms of tool-nose radius compensation.

33. Parameter 1401 LRP and the positioning difference

On the 0i-C the positioning moves of the G70–G76 cycles are made in non-linear positioning regardless of the 1401#1 LRP setting. On the 0i-D the return to the G70 start point is always non-linear positioning; other cycle positioning can depend on the 1401#1 LRP setting. This difference can affect the return path especially near the chuck, on shouldered parts, with large tool holders and in inside-diameter operations; in non-linear positioning the axes move to the end point at independent speeds, so the tool path does not have to be a straight line.

34. G73 and the Series 10/11 program format

The 0i-D parameter manual states that parameters 5135 and 5136 are not used in the Series 10/11 program format. This means that different compatibility formats on the same control unit can handle G73 data with different addresses or assumptions. When a program is taken from another machine, it must be determined whether it is the Series 0 standard format, the Series 10/11 compatibility format, G-code system A/B/C, and whether the builder used a special format.

35. MAJOR DIFFERENCE: G-code system A, B and C

On FANUC lathe controls the G-code system can be A, B or C, and the code of the pattern-repeating cycle can change:

In FANUC tables the G71 function can be shown as G73 on some systems, the G72 function as G74, and the G73 pattern-repeating function as G75 on some systems. Very important: G73 on a machine may not always mean pattern repeating; if G-code system C is used the code can be G75. Also, on machining-centre controls G73 is usually a high-speed peck drilling cycle; the G73 described on this page is for the FANUC lathe system.

36. MAJOR DIFFERENCE: G73 on grinding machines

On FANUC lathe/grinding systems the G71–G74 codes can also be assigned as grinding cycles. On some grinding systems G73 can mean an oscillation grinding cycle or a direct-sizing grinding cycle. On the 0i-D, special grinding options and their selection parameters can change the meaning of the G71–G74 codes. Therefore, before writing G73, it must be verified that the control is a lathe system, that a grinding cycle is not selected, and that the G-code system is appropriate.

37. Commands that must not be used in G73

In the P–Q profile blocks, depending on the control generation, M98, M99, disallowed one-shot G codes, unsuitable group 01 codes other than G00/G01/G02/G03, some group 06 G codes, subprogram calls, interruption-type custom macros, and unsuitable coordinate-system changes cannot be used. The 21i manual states that one-shot G codes other than G04, group 01 codes other than G00/G01/G02/G03, group 06 codes and M98/M99 cannot be used between P and Q.

38. Chamfer, corner R and direct-dimensioning differences

On the old Series 0/00/0-Mate and some 0i-C versions there are restrictions on forming the P–Q profile with chamfer, corner radius and direct drawing-dimension commands; some manuals require these commands not to be used between P and Q. On the 0i-D, chamfer, corner R and direct drawing-dimension input can be used in the profile program; however the last block marked by Q cannot end in the middle of these commands, otherwise PS0326 occurs.

📷 IMAGE AREA — G-code system A/B/C and the lathe / machining-centre / grinding distinction: the different meanings of the G73 code
Suggested alt text: FANUC G73 G-code system and control-type difference

39. G73 alarm solutions

P/S061 — P or Q address missing

P or Q was not specified on the second line of G73. Instead of the faulty G73 P100 U0.4 W0.2 F0.25;, write G73 P100 Q180 U0.4 W0.2 F0.25;. Old FANUC lists state that P/S061 is given when P or Q is missing in the G70–G73 command.

P/S062 — G73 repeat count is zero or negative

G73 U10.0 W4.0 R0; or G73 U10.0 W4.0 R-3; was written. In G73 the R repeat count cannot be zero or negative; on old FANUC systems this error is shown as P/S062. Solution: use a positive integer (e.g. G73 U10.0 W4.0 R4;).

PS0321 — G73 repeat count invalid

On the 0i-D the same error is shown as PS0321 ILLEGAL REPEATED TIME IS IN THE PATTERN REPEATING CYCLE; the cause is a zero or negative G73 repeat count. Solution: check the R on the first G73 line, verify that parameter 5137 is at least 1 if it is used, check the program format, and make sure the R address is not confused with another meaning.

P/S063 — P sequence number not found

G73 P100 Q180 ... was written but N100 may not exist in the program. Check whether N100 really exists, whether N0100/N1000 was written by mistake, whether the P value is correct, whether the same N number is used elsewhere, and whether the profile start was deleted while editing. In old manuals the sequence number specified by P not being found is P/S063.

P/S065 — No G00 or G01 in the first profile block

Instead of the faulty N100 X50.0 Z0.0;, write N100 G00 X50.0 Z0.0; or N100 G01 X50.0 Z0.0;. G00 or G01 must be explicitly commanded in the first profile block of G73 marked by P.

P/S066 — Disallowed G code between P and Q

Causes: another cycle call between P and Q, reference return, an unsuitable coordinate-system change, M98/M99, an unsupported one-shot G code, or an auxiliary move outside the profile. Solution: form P–Q as far as possible only from G00/G01/G02/G03 and move other functions outside the cycle.

P/S067 — G73 called in MDI mode

The G70, G71, G72 and G73 P–Q profile cycles cannot be run in MDI mode on many FANUC controls. Store the program in CNC memory, edit it in EDIT mode and run it in MEMORY/AUTO mode. Issuing a G73 P–Q command in MDI causes the P/S067 alarm.

P/S069 or PS0326 — Profile end not completed

On old systems P/S069: the last move marked by Q may have ended in the middle of a chamfer or corner-R command. On the 0i-D PS0326: the last block ends in the middle of a chamfer, corner R or direct drawing-dimension command. Solution: include the next motion block that completes the geometric command within the Q boundary as well.

PS0324 — Interruption-type macro called while G73 runs

An interruption-type custom macro was called while a G70–G73 cycle was running. Solution: disable the macro interruption during the cycle, check the PMC signal; if it is not visible in the user program, have the machine builder ladder/macro implementation examined.

PS0325 — Unusable command in the profile program

There is a command between P and Q that G73 does not support: M98/M99, another cycle, tool change, an unsuitable G code, a macro call, a coordinate-system change, or a chamfer/direct-dimensioning the control generation does not support must be checked.

PS0327 — G73 called in an unsuitable modal state

On the 0i-D, PS0327 can occur if a modal state in which the G70–G73 cycle cannot run is active. Check: the active tool-nose compensation mode, plane selection, coordinate-transformation functions, polar coordinate interpolation, or the builder special cycle mode. Solution: use a safe start line before the cycle (e.g. G18 G40 G80 G99); however the same start codes should not be used on every machine — the builder G-code structure must be checked.

40. What to check when G73 runs but the tool path is wrong

• G-code system: is pattern repeating really G73? System A/B usually G73, on System C it can be G75.
• Control type: lathe or machining centre? On a machining centre G73 can be a different peck-drilling cycle.
• Grinding option: G73 may be assigned as a grinding cycle.
• First-line U and W: not a single pass but total profile shifts.
• R: not a distance but a repeat count.
• X radius interpretation: the first-line U is usually treated as a radius value.
• Does the raw stock resemble the profile? This is the basic assumption of G73.
• Start point, U/W signs, finishing allowances, tool-nose compensation and the 0i-C/0i-D R1 difference must be checked; if the program omits a value, parameters 5135–5137 must be examined.

41. The most common G73 mistakes

• Thinking G73 is another form of G71; looking for Type I and Type II in G73.
• Thinking the first-line U is a depth of cut, W a finishing allowance, R a retract distance.
• Machining a solid round bar with G73 unnecessarily; writing the cycle without measuring the raw stock shape.
• Thinking the X shift is a diameter value and entering it twice as large.
• Assuming R1 behaves the same on 0i-C and 0i-D; not writing G00/G01 in the P block.
• Running G73 in MDI mode; using M98/M99 between P and Q.
• Overlooking that pattern repeating can be G75 in G-code system C; confusing machining-centre/grinding G73 with lathe G73.
• Copying the 5135/5136 axis counterparts from another control manual.

42. When should a parameter change be considered?

The first solution to a G73 problem is not to change a parameter. First determine the control model and G-code system, check the program format, verify U/W/R on the first G73 line, check the P and Q lines, measure the raw stock shape, examine the start point, run the tool path in graphics and check tool-nose compensation. Only if the program is correct are 5135, 5136 and 5137 examined. A parameter change should be considered only if the value is not given in the program, if the control uses the value modally, if the builder-approved setting is known, and if the old value has been backed up.

43. Preparation before changing a G73 parameter

Record the full model of the control, take a full backup of the parameters, record the current values of 5135/5136/5137 (or 719/720/721 on old Series 0), and photograph the screen. Check the machine builder parameter list, examine whether U/W/R are already given in the program, put the machine in a safe condition and stop the spindle, enable emergency stop, and let only authorised technical personnel make the change.

44. General parameter-change procedure on the 0i-C

Put the machine in MDI mode or enable emergency stop; on the OFFSET/SETTING screen set PARAMETER WRITE to 1 (P/S100 PARAMETER WRITE ENABLE appears). From the SYSTEM/PARAMETER screen go to the number, record the current value, enter the new value with INPUT. Return to the SETTING screen, set PARAMETER WRITE to 0, clear P/S100 with RESET; if a power-off warning appears, turn the CNC off and on according to procedure.

45. General parameter-change procedure on the 0i-D

Switch to MDI mode or enable emergency stop; on the SETTING screen set PARAMETER WRITE to 1 (SW0100 appears). From the PARAMETER screen find the parameter, record the old value and confirm the new value with INPUT; set PARAMETER WRITE to 0 and clear SW0100 with RESET, turn the CNC off and on if a power-off is required, and check the reference/offset/coordinate values. FANUC manuals clearly state that CNC and PMC parameters are set at the factory and should not normally be changed.

46. Safe testing after a parameter change

Turn parameter writing off, clear the alarm, power off/on if required, perform the reference return, check the tool offsets and workpiece zero. Run the G73 program on the graphics screen and examine each profile repeat one by one, dry-run with no tool or part clamped, use machine lock if available. Turn on single block, lower the rapid and feed overrides, observe the stock thickness on the first real pass and the tool load in each region of the profile, and watch the return path. If the result is wrong, restore the old parameter values.

47. The expert operator evaluation order for G73

Before using G73 an expert operator answers: Does the raw stock really resemble the finished profile? Is G73 or G71 more efficient? What is the control G-code system, and is the pattern-repeating code really G73? Is the control 0i-C or 0i-D? Is the first-line U interpreted radially? What are the total X and Z shifts? Is the R repeat count suitable for the tool load, and how does R1 behave by control generation? Is the first shifted profile safe within the raw stock? Can the P–Q profile physically be machined by the tool, and does the tool holder collide on the return? Are the finishing-allowance signs and tool-nose radius compensation correct? Will finishing be done with G70? Only after all of this is it evaluated whether a parameter change is really needed.

48. A short comparison of G71, G72 and G73