By Dana Marshall — Red Seal trades educator with 25+ years in Canadian skilled trades education | Founder, XLR8ed Learning.
You know that G43 turns on tool length compensation. The Red Seal Machinist (429A) exam rarely stops there. It hands you a program block and asks which one activates the offset for a specific tool — and three of the four options look almost right. The mark is lost on one detail: which word tells the control how far to move the Z axis.
This post walks through one commonly missed CNC programming question end to end, so the reasoning transfers to any block the examiner writes. Get this one G43 tool length compensation block right and its variants stop tricking you. It is a companion to our plain-language guide to the G43 tool length offset; here we focus on the exact exam trap — the H-number, and how G44 and G49 sit around it.
The Scenario
You are running a vertical machining centre with a Fanuc-style control. During setup you measured every tool and entered each length in its own offset register. Tool 5 is a drill; its measured length is stored in offset register 5. The tool is already in the spindle after a tool change. The next block has to switch on tool length compensation so the drill reaches the programmed Z depth.
The question: Which block correctly activates the tool length offset for tool 5?
- G43 T05 Z50.0
- G43 H05 Z50.0
- G44 H05 Z50.0
- G49 H05 Z50.0
🎯 RED SEAL RADAR — Machinist (429A)
Maps to Task H-18 (Performs CNC programming) → H-18.02 Creates manual input program, with H-19.02 (Sets up tooling and tool holders) feeding the offset. MWA H (CNC) carries 20% of the exam — or 27 of 135 questions, the third-largest block after lathes and milling. Question type: Procedural/Application. The difficulty driver is a specialist-gap one: manual-trained candidates confuse the H (offset) number with the T (tool) number, or blur G43, G44 and G49, and pick a near-miss. The safest way to solve this type of question is to reason from what the control must do, rather than relying on code recognition alone.
The Short Answer
The correct answer is (b) G43 H05 Z50.0. G43 turns on tool length compensation, and the H word — not the T word — names the offset register whose stored length the control applies to the Z axis. H05 calls register 5, where tool 5’s length was entered during setup. G44 would apply that length in the opposite direction; G49 would cancel compensation instead of activating it.
How do you read a G43 tool length offset question without losing the mark?
Start by reading it the way the exam rewards. This four-step method is the transferable skill; the answer falls out of it.
- Read the whole stem first. The scenario tells you the length lives in register 5 and the tool is already in the spindle. The question is only about activating the offset — not about changing the tool. Options that act on the tool change are off-topic before you compare them.
- Pin down the command word. The word is activates. You are turning compensation on, in the normal direction. That single word rules out G49 (cancel) and pushes back on G44 (opposite direction) before any register number matters.
- Identify every qualifier. “Stored in offset register 5” is the load-bearing qualifier. It points at an H address, because H names the offset register. “Tool 5” is a distractor qualifier — it tempts you toward a T word that does not call the length.
- Predict the answer before reading the options. From memory, the correct shape is: G43, plus the H number that matches the register, on a Z move. You expect G43 H05. Now the options confirm it instead of tempting you.
Worked Reasoning
Tool length compensation exists so you can program the Z axis to the part, not to the machine. The control needs to know how far the tool tip sits from the spindle reference. That distance is the tool length offset, and it lives in a numbered register.
When you command G43 tool length compensation, the control reads the length from the register named by the H word and shifts the Z axis by that amount, so the programmed Z reaches the intended depth. Change the H number and you change which stored length is applied. That is the whole point of the question: the H word is the address, and G43 is the action.
Read the annotated block line by line and the H-versus-T split becomes obvious.
| Program block | What it does |
|---|---|
| T05 M06 | Tool change: puts tool 5 in the spindle. The T word selects the physical tool. It does not apply any length. |
| G43 H05 Z50.0 | Applies tool length compensation. G43 turns it on; H05 calls the length stored in offset register 5; Z50.0 is the target with that length applied. |
| G49 | Cancels tool length compensation before the next tool change. |
Where is the tool length offset stored, and how is it set during setup?
The value comes from setup, not from the program. Under RSOS H-19.02, the machinist determines the required tool offset using methods such as a tool presetter, touching off, measurement, or probing, then enters or confirms that value in the appropriate offset register.
Some shops touch each tool off manually; others use a tool presetter or an in-machine probe that writes the register automatically. Either way, in this Fanuc-style example, the program calls the required offset register with the H word.
In other words, G43 tool length compensation works because setup has already established the tool offset in the register that the H word calls. This is why CNC setup under H-19.02 and CNC programming under H-18.02 are closely related skills.
Distractor Autopsy — why the wrong three fail
Each wrong option is engineered to catch a specific slip. Name the failure and you learn to eliminate it under pressure.
- (a) G43 T05 Z50.0 — tool-number-for-offset-number. This is the trap the whole question is built around. G43 is right, but the T word selects the tool; it does not name the length register. On this control the block needs an H word to apply an offset. Because shops so often set the H number equal to the tool number, the eye accepts T05 as if it carried the length. It does not.
- (c) G44 H05 Z50.0 — direction-code slip. The register is right, but G44 applies the stored length in the opposite direction to G43. With a normal positive tool-length value, G44 shifts Z the wrong way. G44 exists for specific conventions; it is not the everyday turn-on code, and the stem asked to activate compensation in the normal sense.
- (d) G49 H05 Z50.0 — cancel-for-apply. G49 cancels tool length compensation. Adding H05 does not turn G49 into an activation command; the stem asks to apply the offset, not cancel it
Exam Curveball
Change one word and the answer moves. Same machine, same register — but now the program has finished the drill and has to cancel tool length compensation and retract Z before the next tool change. Which code is correct now?
The answer becomes G49 (or H0 on controls that read it as a zero offset). One changed qualifier — activate versus cancel — flips the correct code from G43 to G49. Memorising “the answer is G43 H05” fails here; understanding that G43 applies and G49 cancels does not.
📋 STANDARDS & REFERENCE COVERAGE
RSOS Sub-task: H-18.02 Creates manual input program (primary); H-19.02 Sets up tooling and tool holders on CNC machines (secondary — where the offset is measured and stored).
Trade: Machinist — Red Seal (Ontario 429A).
Standards / references: ISO 6983 (G-code / RS-274) — the numerical-control programming language. The exact behaviour of G43, G44, G49 and the H/T relationship is CNC-control-specific (Fanuc-style is shown here); confirm against the machine’s control programming manual and the governing drawing before you rely on it.
Manufacturer / data basis: Yes — the control builder’s programming manual governs the precise word behaviour, so treat “per the control documentation” as the operative authority, not a generic rule.
Provincial / OHS note: Machine guarding and interlocks under CSA Z432 and O. Reg. 851 (Industrial Establishments); control of hazardous energy under CSA Z460 for tooling changes and reaching into the enclosure.
Contested-reading note: G-code dialects vary by control. This post uses the common Fanuc-style convention where G43 shifts in the positive sense and H addresses the offset register. On a control whose manual defines these words differently, verify before teaching a candidate the block is universal.
Frequently Asked Questions
What is the difference between G43, G44 and G49 on the Red Seal machinist exam?
G43 turns on tool length compensation and shifts the Z axis by the length stored in the offset register you name with the H word, so the programmed Z reaches the correct depth. G44 applies that same stored length in the opposite direction and is used only with specific setup conventions. G49 cancels tool length compensation. On controls that treat H0/H00 as a zero-offset cancellation, H0/H00 may also remove the effective tool-length compensation; confirm this in the control manual. On the exam, treat G43 as the everyday turn-on code, G44 as the rare opposite-direction case, and G49 as the cancel. Confirm the exact behaviour against your control’s programming manual.
How does the H number relate to the tool number when you apply G43?
The H number addresses the offset register that holds a tool’s length; the T number selects the physical tool. They are separate. Many shops set the H number equal to the tool number by convention, so tool 5 uses H05. The H and T addresses perform different functions, although some controls or machine settings can require their numbers to match When you write G43, the H word, not the T word, tells the control which stored length to apply to the Z axis. Calling the wrong H number applies the wrong length even when the right tool is in the spindle.
What happens to the Z axis if you call G43 with the wrong H number?
The control shifts the Z axis by whatever length is stored in that register, not the length of the tool actually in the spindle. If the stored value is larger than the real tool length, the tool stops short and cuts air; if it is smaller, the tool drives past the programmed depth and can crash into the part, the fixture, or the table. Prove out every new tool with a dry run and single-block mode before running at rapid so a wrong H number is caught in the air, not in the steel.
Why This Matters On The Job
A wrong or missing tool length offset is not an abstract exam slip — it drives the Z axis to the wrong place. Too little offset and the tool can travel past the intended programmed depth into the workpiece, fixture, or table, potentially damaging or shattering tooling. That is why setters prove out a new program using methods such as a dry run, single-block mode, and reduced feed and rapid overrides before running at full speed.
Machine guarding and interlocks help control the hazards associated with CNC machining (CSA Z432 and O. Reg. 851): the enclosure keeps the operator separated from moving machinery while containing chips and coolant. Before entering a machine hazard zone for setup, measurement, adjustment, or tooling work, follow the machine manufacturer’s safe procedure and the workplace’s energy-control requirements. Where unexpected startup or movement could endanger the worker, apply the required lockout/tagout procedure. Getting G43 and the H-number right protects the part, the machine, and the person standing at the pendant.
Tailgate Checklist
- ✓ The H word addresses the offset register; the T word selects the tool. Same number by habit, different jobs.
- ✓ G43 applies, G44 applies the opposite direction, G49 cancels. Read the command word — activate or cancel — first.
- ✓ Wrong H number equals wrong Z equals a possible crash. On the job, prove out; on the exam, check the register matches.
- ✓ RSOS H-18.02 pairs with H-19.02: the program names the register, but setup put the length in it.
- ✓ G-code behaviour is control-specific — for a real machine, confirm G43 tool length compensation against the control’s programming manual.
Own the Reasoning, Not Just the Answer
Don’t leave your certification to chance. Unlike standard courses, XLR8ed Learning offers a Commitment to Completion (C2C) Plan. We provide 10 weeks of initial access to our mobile-optimised quizzes and lessons. If you are unsuccessful with your exam attempt, we provide you 4 weeks of access prior to each additionally required exam attempt at no charge. We are in this with you until you get that Red Seal.
This article references the current Red Seal Occupational Standard for Machinist (429A). G-code behaviour, including G43, G44, G49 and offset-register logic, depends on the specific CNC control and the governing engineering drawing; always confirm behaviour against the machine’s control documentation before relying on it. Authorities: Red Seal Program — Machinist, CSA Group (Z432, Z460), and Skilled Trades Ontario.
For more articles or Red Seal Machinist (429A) exam questions, check out our Machinist Hub.