📷 IMAGE AREA — M70/M700 fixed cycle (G83) screen: Z, R, Q, F addresses and the pecking motion
Recommended size: 1200×630 px (16:9, hero) · WebP/JPG · <150 KB · filename: mitsubishi-m70-g83-fixed-cycle.webp · alt: Mitsubishi M70 G83 peck drilling fixed cycle screen Z R Q F
On the Mitsubishi M70 the word “parameter” is used in two different senses that must not be confused. Process values written in the program (addresses such as Z, R, Q, F on a G83 line) can be changed by the operator or programmer according to the job. In contrast, the machine parameters of the control (CNC settings such as #8013 G83 return, #2109 Rapid or #8033 Smoothing) affect the working character of the machine and must not be changed without the manufacturer’s approval. This guide explains M70 program and system settings from fixed-cycle addresses to high-speed high-accuracy die-machining parameters, staying faithful to the source manual.
1. Basic addresses in fixed drilling cycles
The basic addresses used in fixed cycles such as G73, G81, G82, G83, G84 on the Mitsubishi M70 are:
| Address | Function |
|---|---|
| X, Y | Position of the hole center |
| Z | Final depth of the hole |
| R | Approach plane where rapid changes to cutting feed |
| Q | Amount taken per peck or step |
| P | Dwell time at the hole bottom |
| F | Cutting feed or tapping pitch |
| L | Number of cycle repeats |
| G98 | Return to initial level at cycle end |
| G99 | Return to R plane at cycle end |
| G80 | Cancel the fixed cycle |
The Mitsubishi programming manual defines Q as the amount taken per cut for G73 and G83, R as the approach plane, Z as the hole end and L as the number of repeats.
2. G83 deep-hole peck drilling
G83 retracts the drill at set intervals in deep holes so that chips can clear. The general form is G98 G83 X.. Y.. Z.. R.. Q.. F...
G90 G54 G0 X20. Y30.
G43 H3 Z50.
G98 G83 Z-40. R2. Q5. F120.
G80In this example the hole center is X20 Y30, the hole end Z-40, the approach plane R2, the peck amount Q5, the feed F120, and G98 returns to the initial level at hole end. The Q value defines how many millimeters the drill advances on each cutting move; Q5. means the drill advances in roughly 5 mm steps (drill 5 mm, retract, drill 5 mm more…). Q is always treated as an incremental amount; even with G90 active, Q5 does not mean absolute position Z5 — it is the depth per peck.
A single fixed Q value is not correct for all jobs. The main factors affecting the choice of Q are: drill diameter and length, hole depth, workpiece material, whether coolant reaches the hole, chip shape, whether the drill is carbide or HSS, and whether through-coolant is present. General logic: if chips clear easily, Q can be larger; if chips jam, reduce Q; for a thin, long drill, prefer smaller steps; as depth increases, pay more attention to chip evacuation. Increasing Q only to speed up production can cause drill breakage and hole jamming.
3. How is the G83 retract amount set? (#8013)
G83 has two distinct motions. Full retract: after each peck the drill rapids up to the R plane or the return level defined by the cycle; this is the basic feature of G83. Approach distance to the previous cut level: when the drill re-enters the hole it does not travel the whole distance at cutting feed; it first rapids to near the previously machined level, then switches to cutting feed for the last few millimeters. This few-millimeter safety distance is set on the Mitsubishi M70 by the #8013 G83 return parameter. The manual denotes it with the letter m and gives the condition Q > m: the peck amount in the program must be greater than the approach distance in #8013.
Example: Q = 5 mm, #8013 = 1 mm. The first peck is 5 mm. On the second peck the drill retracts to clear chips, rapids to about 1 mm before the previously machined level, covers the last 1 mm at cutting feed and performs the new 5 mm peck. If this distance is too small the drill can rapid too close to the hole bottom; too large and time is wasted on each peck; equal to or larger than Q and the cycle logic can break down. #8013 is not an ordinary program setting; it affects the general cycle behavior tested by the machine manufacturer. If retract must be changed only for a specific hole, Q, R, feed and tool conditions should be evaluated first.
4. Difference between G73 and G83
G73 is also a step-drilling cycle, but its retract motion is not as large as G83’s. In G73 the drill retracts a short amount at each step; it suits relatively shallow holes, materials where chips break easily and jobs needing a faster cycle (e.g. G73 Z-20. R2. Q3. F150.). The short retract of G73 is set by the #8012 G73 return parameter. In G83 the drill retracts more to clear chips; it suits deep holes, long-chip materials and holes with a high chance of chip jamming.
| Feature | G73 | G83 |
|---|---|---|
| Retract | Short | Wider/full |
| Cycle time | Shorter | Longer |
| Chip evacuation | Medium | Better |
| Deep hole | Limited | More suitable |
| Related parameter | #8012 | #8013 |
5. G81 simple drilling cycle
The general form is G81 X.. Y.. Z.. R.. F.. (e.g. G99 G81 X20. Y20. Z-12. R2. F180.). In G81 there is no pecking; the drill goes from the R level to the Z level in one cutting move, there is no dwell at the hole bottom, and it then returns per G98 or G99. It is used for shallow holes, spot drilling and jobs with no chip-evacuation problem. Q is not used in G81.
6. G82 dwell drilling and flat counterbore
The general form is G82 X.. Y.. Z.. R.. P.. F.. (e.g. G82 X40. Y30. Z-5. R2. P500 F100.). P is the dwell time at the hole bottom; the dwell can clean the base of a flat counterbore, reduce the tool mark and improve the bottom quality of the hole. However, the time unit and decimal usage of P must be verified against the control setting; the manual states that the decimal part of the P address is ignored in fixed cycles.
7. G84 tapping cycle (#8018)
The general use is G84 X.. Y.. Z.. R.. F... In synchronous tapping the F value is mostly used according to the thread pitch; for M8×1.25, e.g. S500 M3 / G84 Z-18. R3. F1.25. However, in some control configurations the meaning of F (feed per revolution, feed per minute, synchronous/asynchronous tapping selection) can depend on settings. On the M70, synchronous or asynchronous tapping selection can be determined by additional address and control parameters in the program; therefore a G84 line taken from another brand of control must not be used directly.
The M70 programming manual has a step or peck tapping form for G84 and G74: G84 X.. Y.. Z.. R.. Q.. F.. P.. S... Here Q is the amount the tap advances each pass, P the dwell, S the spindle speed, F the tap pitch or the feed per the chosen method. The tap can retract at each Q distance to reduce load. The retract amount in this cycle can be set by the #8018 G84/G74 return parameter, and whether the step tapping cycle is active can be related to the #1272 ext36/bit0 parameter. This bit is not an ordinary operator setting; it must not be changed without considering the manufacturer’s synchronous tapping structure, the spindle drive and the PLC logic.
8. G98 and G99 setting
Where the tool returns at the end of a fixed cycle is set by these two modal G codes. In G98 the tool returns to the initial level from before the cycle (e.g. G0 Z50. / G98 G83 Z-30. R2. Q5. F100. → the tool returns to Z50 at hole end). This choice is safer when passing over a vise, over tall clamps, or when there are obstacles between parts. In G99 the tool returns only to the R level (e.g. G99 G83 Z-30. R2. Q5. F100. → the tool returns to R2 at hole end); it reduces time on multiple holes but can come near a vise or clamp while moving between holes. The manual notes that the control’s initial state can be G98 and that G98/G99 are modal.
9. How is the R plane selected?
The R value is the safe plane where the tool changes from rapid to cutting feed. For example R2. can mean switching to cutting feed 2 mm above the Z0 top surface of the part. When selecting the R level, consider burr on the part surface, curvature of the part, fixture height, tool approach safety and G90/G91 usage. If R is too high the cycle slows down; if R is too low the tool rapids too close to the part.
10. Effect of G90 and G91 on fixed cycles
In G90 absolute programming (e.g. G90 G83 Z-30. R2. Q5.) Z and R are treated as positions relative to the active workpiece zero. In G91 incremental programming (e.g. G91 G83 Z-30. R-3. Q5.) Z and R are treated as incremental moves relative to the start position. Using G91 in fixed cycles requires more care; a wrong R sign can make the tool move in an unexpected direction. Q, however, is treated incrementally as the peck amount independently of G90/G91.
📷 IMAGE AREA — High-speed high-accuracy die machining (G05.1 Q1 / G05 P10000) tool path and corner control
Recommended size: 1000×750 px (4:3, in-content) · WebP/JPG · <150 KB · filename: mitsubishi-m70-high-speed-accuracy-die.webp · alt: Mitsubishi M70 high speed high accuracy die machining G05.1 tool path
11. Are there Type 1 and Type 2 modes in die machining?
Yes. The Mitsubishi M70 programming manual has two separate high-speed high-accuracy control modes for die and high-speed surface machining. These are not the same as Program Restart Type 1 and Type 2. High-speed high-accuracy control I: open G05.1 Q1, close G05.1 Q0. High-speed high-accuracy control II: open G05 P10000, close G05 P0. These two modes cannot be used at the same time. So “Type 1 and Type 2 in die machining” actually corresponds in the manual to high-speed high-accuracy control I and II; this is a completely different subject from the restart method.
12. Basic difference between die machining mode I and II
The purpose of both modes is to process the many short G01 blocks coming from CAM more smoothly, to decelerate appropriately at corners, to pre-calculate servo acceleration and deceleration, and to balance surface quality against machining time. According to the manual, Mode I evaluates a limited number of look-ahead blocks on fine segments; Mode II evaluates more blocks in advance and offers more advanced path-processing features. Mode II has extra functions such as smoothing, an acceleration clamp and corner control that takes short segments into account.
| Mode | General use |
|---|---|
| Mode I (G05.1 Q1) | More basic high-speed and smooth surface machining |
| Mode II (G05 P10000) | Dense CAM blocks and more advanced die-machining control |
However, it should not be assumed that Mode II is present on every M70 machine; these features can be optional.
13. Option and parameter needed for G05.1 and G05
The manual states that high-speed high-accuracy control I and II are optional functions. If the option is absent, G05.1 Q1 or G05 P10000 can cause a program error. The function is also related to the #1267 ext03/bit0 parameter. An option that has not been purchased cannot be enabled by changing this parameter; the function must be present in the control software, the option license and the machine settings.
14. Modal states required when entering die mode
Before switching to high-speed high-accuracy mode some functions must be off. Important conditions given in the manual: G40 cutter radius compensation cancel, G49 tool length compensation cancel (especially under Mode I conditions), G50.1 programmable mirror cancel, G67 modal macro call cancel, G69 coordinate rotation cancel, G80 fixed cycle cancel, G94 feed per minute, G97 constant surface speed cancel. A suitable cutting mode must also be used. If G05/G05.1 is given without meeting the conditions, program errors such as P34 can occur.
G40 G49 G80
G69
G94
G05.1 Q1
...
DIE SURFACE MACHINING BLOCKS
...
G05.1 Q0The open and close commands must be written on independent lines.
15. Can other commands be written on the G05/G05.1 line?
According to the manual the open and close lines must be independent. Correct: G05.1 Q1. Wrong example: G05.1 Q1 G1 X100. F2000. Using an address other than G/Q or G/P can cause a program error. A decimal point must not be used either: Q1 is correct, Q1.0 must not be used.
16. High-accuracy control: G61.1 and G08
In die machining, besides G05/G05.1 there is also a more basic high-accuracy mode. G61.1 (G61.1 F..) turns on high-accuracy control; to cancel, a G code from the same group such as G64 can be used. G08 (G08 P1 turns on, G08 P0 cancels) must be written on an independent line. These modes apply pre-interpolation acceleration and deceleration control so that motion occurs closer to the commanded path.
17. Basic speed parameters in high-accuracy mode (#2109, #2110)
#2109 Rapid (H-accuracy) sets the rapid traverse speed used during high-accuracy mode; if #2109 = 0 the control can use the general rapid parameter #2001 rapid. #2110 Clamp (H-accuracy) sets the upper limit that cutting feed can reach during high-accuracy mode; if #2110 = 0 the general cutting speed limit #2002 clamp can be used. These parameters relate directly to surface quality, cycle time and the machine’s acceleration behavior. Raising the value does not always give a better result; if the machine’s mechanical rigidity and servo tuning are insufficient, corners can round off, surface waviness can appear, vibration can increase and servo following errors can occur.
18. Acceleration parameters (#1206, #1207)
Some important parameters in high-accuracy control are #1206 G1bF and #1207 G1btL. According to the manual the allowed acceleration relates roughly to the ratio of these values: Allowed acceleration = #1206 / #1207. #1206 relates to the target speed and #1207 to the time to reach the target speed. These relate directly to servo and machine dynamics and must not be changed at random by the operator just to machine a surface faster.
19. Die-machining parameters of Mode II (#8029–#8037)
- #8033 Smoothing ON: 0 = smoothing off, 1 = smoothing on. The smoothing function can be used to smooth very short zigzag G01 paths produced in the CAM program; it is valid only on continuous linear G01 blocks.
- #8029 Smoothing L: sets the length limit of the short protrusion to be smoothed. Segments shorter than this value can be smoothed; if set too high, the real part geometry can change more than intended.
- #8034 AccClampt ON: 0 = normal speed and corner deceleration control, 1 = speed limiting per the acceleration decision. Especially on surfaces that continue with small angle changes but have generally sharp curvature, it limits the speed according to the machine’s acceleration capacity.
- #8036 CordecJudge: sets how short segments are evaluated in the corner deceleration decision. 0 = decide by the direct angle of adjacent blocks, 1 = decide while excluding very short blocks.
- #8037 CorJudgeL: sets the segment length considered a “very short block” in the corner decision. It can prevent very small blocks in the CAM program from needlessly disturbing the corner speed.
20. Curve and corner accuracy parameters (#8019–#8023)
The manual also has these die-machining corner and arc parameters: #8019 R COMPEN related to accuracy or speed compensation on circular moves; #8020 DCC ANGLE related to corner connection and angle criterion; #8021 COMP CHANGE accuracy-coefficient change behavior; #8022 CORNER COMP corner compensation; #8023 CURVE COMP curve compensation. These affect part geometry, program block length, speed and servo behavior together. Changing these settings can change the corner size, the circle diameter, the surface mark and the machining time; setting them without a manufacturer test part and measurement method is not correct.
21. G05.1 Q2 is not Mode II
This distinction is important. G05.1 Q1 is high-speed high-accuracy control I. But G05.1 Q2 is used in the manual for the spline function. The command for high-speed high-accuracy control II is G05 P10000. So they should be separated as: G05.1 Q1 = high-speed high-accuracy I, G05 P10000 = high-speed high-accuracy II, G05.1 Q2 = spline function.
22. G05.1 Q2 spline function parameters (#8025–#8030)
The spline function can be used to create a smoother curve from short linear segments in the CAM program. Open example G05.1 Q2 X0 Y0 Z0, close G05.1 Q0. Some related parameters: #8025 SPLINE ON enable the spline function; #8026 CANCEL ANG. the angle limit at which the function is cancelled; #8027 Toler-1 first tolerance; #8028 Toler-2 second tolerance; #8030 MINUTE LENGTH short-segment length limit. This function can change the part path directly; it must not be enabled without knowing the die surface tolerance.
23. Which setting does the programmer change, which the service?
Values the programmer or authorized operator can set by the job: G83 Z depth, R approach plane, Q peck amount, F feed, G98/G99, the choice of G73 or G83, G84 pitch and depth, opening and closing G05.1 or G05 in the appropriate program, tool/speed/coolant values.
Values that must be set by the manufacturer or an expert: #8012, #8013, #8018, #1206, #1207, #1267, #1272, #2001, #2002, #2109, #2110 and the high-accuracy and die parameters in the #8019–#8037 range. These parameters can affect not only a single program but all programs using the same function.
24. Method to apply before changing a parameter
- Record the current parameter value and take a parameter backup.
- Verify from the manual which function the change affects.
- Check the lower and upper limits recommended by the machine manufacturer.
- Change only one parameter, by a small amount, at a time.
- Run the test part at low feed and a low rapid rate.
- Compare dimensions and surface quality; monitor servo load, vibration and noise.
- If the result worsens, return to the old value.
A parameter appearing on the screen does not mean the operator is authorized to change it.
25. Application examples
G83 for a deep hole:
G90 G54 G0 X25. Y20.
G43 H5 Z50.
S1200 M3
M8
G98 G83 Z-45. R3. Q5. F110.
G80
G0 Z100.
M9
M5Things to check: is Q5 suitable for the drill and material? Is R3 safe from the part surface? Is G98 needed? Is #8013 smaller than Q? Does coolant reach the hole?
G99 for multiple holes:
G90 G54
G0 X20. Y20.
G43 H4 Z30.
G99 G81 Z-12. R2. F160.
X50.
X80.
Y50.
G80
G0 Z50.It must be certain that there is no clamp between the holes at the R2 level.
Entering die surface machining:
G40 G49 G80
G69
G94
G05.1 Q1
G1 X... Y... Z... F...
G1 X... Y... Z...
G05.1 Q0After closing the mode, return to normal program commands.
Conclusion
On the Mitsubishi M70 the way G codes work does not depend only on the values on the program line. In G83, Q is the cut amount per peck, R the approach plane, Z the hole end, F the feed, and #8013 the safety approach distance to the previous cut level. In die machining, G05.1 Q1 is high-speed high-accuracy control I, G05 P10000 control II, and G05.1 Q2 the spline function. Mode I and Mode II are not merely a different software option; the CNC option, control parameters, servo tuning and program commands work together. If the machine does not have the option, these functions cannot be used just by changing parameters.
⚠️ Mentor CNC — safety and responsibility note: This content is prepared for general educational purposes. Even with the same Mitsubishi M70/M700 control, the behavior of fixed cycles, spindle synchronization, high-speed machining options, servo settings and parameter values can vary by machine manufacturer. Parameters such as #8012, #8013, #8018, #1206, #1207, #1267, #1272, #2109, #2110 and #8019–#8037 must not be changed without the manufacturer’s approval. A wrong setting can cause drill or tap breakage, dimensional error, surface defect, servo alarm and collision. Mentor CNC is not responsible for any damage arising from applications; parameter changes must be made under the supervision of an authorized CNC expert or the machine manufacturer.