📷 IMAGE SLOT — Diagram of the G83 peck drilling cycle showing the Q step and the retract distance · Suggested size: 1200×630 px (16:9, hero) · WebP/JPG · <150 KB · file name: mitsubishi-m70-g83-peck-drilling-retract.webp · alt: Mitsubishi M70 G83 peck drilling cycle retract distance and Q step depth
On a machining centre with a Mitsubishi M70 or M80 control, the peck steps when drilling, the stepped infeed when tapping, and above all their retract distances are not set in the program — they are set in the control’s parameters. This page covers exactly that: which parameter does what, what happens when you increase its value, and what happens when you decrease it.
The basic distinction: the Q you write in the program says how far the tool goes down on each step. The parameters say how the tool behaves between those steps. One does not replace the other.
Quick Reference: What Are You Trying to Change?
| What you want to change | Setting | Applies to |
|---|---|---|
| How far the tool feeds down on each step | Q (in the program) | Drilling and tapping |
| Retract distance at the end of each G73 step | #8012 | Drilling |
| Rapid-to-feed (safety) clearance in G83 | #8013 | Drilling |
| Stop G83 returning to R on every step | #8115 | Drilling |
| Retract distance at the end of each tapping step | #8018 | Tapping |
| Which stepped-tapping type is active | #1272 ext36/bit0 | Tapping |
1. Peck Drilling: The Difference Between G73 and G83
Both cycles drill the hole in steps rather than in one plunge. The only difference is how far the drill retracts at the end of each step:
- G73: the drill backs off only a short distance and stays inside the hole. Its purpose is to break the chip. It is fast, and suits short-chipping materials.
- G83: the drill returns all the way to the R plane on every step, so it comes right out of the hole. It clears the chips completely. Safer but slower, and suits deep holes and long-chipping materials.
#8012 — retract distance in G73
What it does: sets how many millimetres the drill backs off at the end of each G73 step. Setting range: 0 to 99999.999 mm.
- Increase it: the drill backs off further, the chip breaks and clears more easily. Cycle time goes up slightly.
- Decrease it: the cycle gets shorter. But if the retract is too small to break the chip, the flutes pack up, the hole finish suffers and the drill is overloaded.
#8013 — rapid-to-feed clearance in G83
What it does: in G83, after the drill has returned to R and plunges again, it does not rapid (G00) all the way down to where the previous step ended. A few millimetres before that depth it drops out of rapid into cutting feed (G01). #8013 sets how far ahead of that depth the change happens. Setting range: 0 to 99999.999 mm.
- Increase it: the drill slows down earlier. Less risk of rapiding into chips left at the bottom and snapping the point. Cycle time goes up.
- Decrease it: the cycle gets faster. But if chips remain at the bottom, the drill rapids straight into them and the risk of breaking the point rises.
Rule you must follow: the Q value in the program has to be larger than the value set in #8013. The depth taken per step can never be smaller than the clearance distance.
#8115 — should G83 return to R at the end of each step?
What it does: selects the motion after each step completes in the G83 (deep-hole drilling) and G87 (back boring) cycles. There are two options:
- 0 (normal): the tool returns all the way to the R plane after every step. Classic G83 behaviour.
- 1: the tool does not climb back to R; it backs off by a set amount and carries on. The cycle speeds up, behaving much like G73.
When this helps: if your complaint is “my G83 climbs back to R every single time and I am losing cycle time, I want a short retract like G73”, you do not need to rewrite the program as G73 — setting this parameter to 1 is enough.
2. Stepped Tapping (G84 and G74)
First, the terminology. The Mitsubishi manual calls this “pecking tapping”. On the shop floor people say “stepped tapping” or “peck tapping”. They all mean the same thing: the tap cuts the thread in several steps instead of one continuous pass. The purpose is to reduce the load on the tap in deep holes and stop it from breaking.
How do you switch stepped tapping on?
You add a Q to the G84 (right-hand thread) or G74 (left-hand / reverse) block. Q is how far the tap advances on each step:
G84 X20. Y20. Z-30. R3. Q5. F500.
( Q5 = the tap advances in 5 mm steps )If you omit Q from the block, or command Q0, the cycle runs as normal single-pass tapping. So if you do not want stepped behaviour, simply leave Q out of the block.
There are two types of stepped tapping — worth knowing
The manual defines two separate forms of stepped tapping, and which one your machine performs is selected by parameter:
| Step type | What the tap does | When it is preferred |
|---|---|---|
| Short retract (manual: pecking tapping) | Backs off a short distance inside the hole at the end of each step; never leaves the hole | When simply reducing load is enough; this is faster |
| Full return to R (manual: deep-hole tapping) | Returns all the way to the R point at the end of each step, leaving the hole completely | When chips and coolant need clearing; safer but slower |
The choice between the two is made by #1272 ext36/bit0. This is not an operator setting — it involves the machine’s synchronous tapping arrangement, the spindle drive and the PLC logic. If it needs changing, talk to the machine builder or an authorised service engineer.
#8018 — retract distance at the end of each tapping step
What it does: in the short retract type from the table above, it sets how many millimetres the tap backs off at the end of each step. Setting range: 0 to 999.999 mm.
- Increase it: the tap backs off further, chips and lubricant move more freely at the thread root, and the load on the tap drops. Cycle time goes up.
- Decrease it: the cycle gets shorter. But if the retract is too small, the benefit of stepping is lost and the tap stays overloaded.
- Set it to 0: the cycle behaves like normal single-pass tapping.
3. Before You Change Any Parameter
- Take a backup. Write down the existing value before changing it, and if possible back up the whole parameter set to a CF card or USB stick.
- If you do not know, do not touch it. Never change a parameter you are unsure of just to see what happens — ask someone qualified.
- Change it in small steps. Work up gradually and observe the result instead of making one large change.
- Run the first hole in single-block mode. Use a low feed override and keep your hand on the stop button.
- Make sure you are in the right group. These are machining parameters. Never touch servo, spindle or safety parameters.
- They may be locked. The machine builder may have locked certain parameters. Do not force it — contact the authorised service.
4. Symptom – Where to Look
| What you are seeing on the machine | Where to look |
|---|---|
| G83 is very slow, slowing down far too early on every step | Reduce #8013 carefully |
| The drill rapids into chips at the bottom and the point breaks | Increase #8013 |
| In G73 the drill retracts but the chip never breaks | Increase #8012 |
| G83 keeps climbing back to R and the cycle drags | Set #8115 = 1 (back up first) |
| The tap is struggling or breaking in deep holes | Add Q to the G84 block to run it stepped, then tune #8018 |
| I added Q but the tap is not running stepped | #1272 ext36/bit0 may not be set correctly — ask your service engineer |
| It runs stepped, but chips and coolant are not clearing the hole | The full-return-to-R type is needed (#1272) — ask your service engineer |
Common Mistakes
- Confusing Q with the parameter. Q is the step depth and is written in the program; the retract distance is a parameter.
- Programming a Q in G83 that is smaller than the value in #8013.
- Shrinking #8013 to save time while ignoring the risk of rapiding into packed chips.
- Entering a parameter number published for a Fanuc control into a Mitsubishi machine. The numbers are control-specific.
- Changing parameters without taking a backup.
- Experimenting with system bits such as #1272 at operator level.
Do Not Mix These Up With Fanuc Numbers
The G-codes themselves (G73, G83, G84) mean much the same thing on almost every control. But the parameter numbers that govern how those codes behave differ from brand to brand and series to series. On a Fanuc, the equivalent settings live under completely different numbers. The numbers on this page apply only to the Mitsubishi M700/M70 and M800/M80 series. Before entering any number you found online, confirm which control it was written for.
Summary
In drilling you program the peck step with Q, while the behaviour between steps is governed by #8012 for G73 and by #8013 and #8115 for G83. In tapping you switch stepped operation on by adding Q to the G84 or G74 block; #8018 sets the retract distance at the end of each step, and #1272 ext36/bit0 decides which form that step takes — a short retract or a full return to R. Whatever you change, the order is always the same: back up, change in small steps, prove it in single block.
Mentor CNC Disclaimer and Safety Notice
This content was prepared for training purposes based on the official Mitsubishi M700/M70 programming manual and the official Mitsubishi M800/M80 series parameter manual. Parameter behaviour may differ depending on the NC software version and the machine builder’s configuration. Parameter changes and stepped-cycle trials cause real tool and machine motion; they must not be applied without a backup, without the supervision of a qualified person, and without first proving the cycle in single-block mode at low feed. For definitive information, always refer to your machine’s parameter manual and the machine builder’s documentation.