Machinist CNC programming, set-up and operation practice questions (429A).

Five free practice questions on CNC programming, set-up and operation: block H of the Red Seal 429A Machinist exam, about 27 of its 135 questions. They are in the exam's format: four options, one correct answer. Answer each one before opening the explanation. No account, no email.

01The questions

1. Procedural · Creates manual input program

   Where in a milled profile program should G41 with its D number be programmed?

   1. On a straight lead-in longer than the cutter radius.
   2. On the first cutting move along the edge of the part.
   3. On the first arc of the profile itself.
   4. On the Z move that feeds the cutter down to depth.
   Show the answer

   A. Correct. Compensation is switched on in a linear move, clear of the part and at least a cutter radius long, so the control can shift the tool sideways by the radius before it touches the contour. G40 cancels it on a lead-out after leaving the part.

   Why not the others

   B. The control builds the offset up during the start-up move, so the first edge would be cut on a slant, gouged or undercut. Switch it on during a lead-in clear of the part.

   C. Most controls will not start compensation on an arc and stop with an alarm, and any that did would gouge the contour while the offset built up. It belongs on a straight lead-in before the profile.

   D. A Z-only move has no motion in the XY plane to build the offset in, so on many controls the offset is applied on the next XY move, which is the first cut. Use a separate straight lead-in in X and Y.

2. Recall · Creates manual input program

   On a machining centre, a G02 arc moves in X and Z only and is programmed with its centre, not a radius. Which plane code must be active, and which words give the arc centre?

   1. G19, with J and K.
   2. G17, with I and K.
   3. G18, with I and K.
   4. G17, with I and J.
   Show the answer

   C. Correct. G18 selects the ZX plane, and the centre words follow the axes: I goes with X, J with Y and K with Z, so an arc in X and Z takes I and K. Switch back to G17 before any XY arcs or cutter compensation in the XY plane that follow.

   Why not the others

   A. G19 with J and K is the pair for an arc that moves in Y and Z, such as a radius milled across a part along Y. This arc moves in X and Z, so it needs G18 with I and K.

   B. I and K are the right centre words for an arc in X and Z, but G17 leaves the control in the XY plane, where arcs are cut in X and Y. The plane has to be switched to G18 before the arc.

   D. G17 is the XY plane that most machining-centre programs start in, and I and J are its centre words. This arc moves in X and Z, so it needs the ZX plane, G18, with its centre given by I (along X) and K (along Z).

3. Procedural · Establishes work datum

   The X, Y and Z work offset for a vise job has just been entered in the register. How is it checked before the program is run?

   1. Zero the relative position display at the datum corner.
   2. Check that the values match the last job's offsets.
   3. Run the program in graphics, which shows the datum position.
   4. Move a tool over the datum corner at a safe height in MDI.
   Show the answer

   D. Correct. A commanded move with the new work offset active, to X0 Y0 well above the part, shows directly whether the spindle lands over the datum corner. A sign error, a swapped axis or a typing slip shows up as a tool in the wrong place instead of a crash.

   Why not the others

   A. The relative display is a scratch counter for the operator; zeroing it changes nothing in the work offset and checks nothing.

   B. A new set-up puts the vise and part somewhere else; the old offsets prove nothing about the values just entered.

   C. Control graphics plot the program in its own coordinates; they do not know where the real part sits on the table, so a wrong offset looks perfect on screen.

4. Recall · Verifies program

   During prove-out the feed override is at 10 %, yet the approach to the part still comes in fast. On this control the feed and rapid overrides are separate. What is the cause?

   1. Overrides work only with single block turned on.
   2. The override acts only once the tool is in the material.
   3. The approach is a rapid move under the rapid override.
   4. The F word in the block takes priority over the override.
   Show the answer

   C. Correct. G00 moves run at the machine's rapid rate, scaled by the rapid override (usually in fixed steps down to a slow creep), not by the feed override. On a first run both are turned down before the approach.

   Why not the others

   A. Overrides act in automatic operation whether single block is on or off; single block only makes the machine stop at the end of each block.

   B. The feed override scales every feed move, G01, G02 and G03, from the moment it runs, in or out of the material; it simply does not apply to rapids.

   D. The override is a percentage of the programmed F; at 10 % a feed move runs at a tenth of F. A fast approach under a low feed override points to a rapid move.

5. Procedural · Restarts program cycle

   A program was stopped during tool 4's roughing pass, and the cause has been fixed. Where should the restart begin?

   1. At the block where the cycle stopped.
   2. At tool 4's safe-start block at its tool change.
   3. At tool 4's first feed move, with the spindle started in MDI.
   4. At tool 5's tool change, leaving tool 4's work for later.
   Show the answer

   B. Correct. The tool-change block and the lines after it call the tool, its length offset, the work offset, spindle speed and coolant, so every modal setting is restored before the tool approaches. Already-cut areas are passed through in air, which costs a little time and nothing else.

   Why not the others

   A. After a reset, starting at the stopped block skips the earlier lines that set the offsets, speed and coolant, so the tool can move without them.

   C. Starting partway into the tool with the spindle set by hand skips the blocks that call the length offset, work offset and coolant; one missed setting can crash the tool.

   D. Skipping to tool 5 leaves the roughing unfinished, so later tools meet full stock they were not programmed to cut.

02Answer key

03What block H covers

Block H is CNC machining on machining centres and turning centres. Programming covers process documentation, manual G-code programs, canned cycles, cutter radius compensation, tool length offsets, program transfer and editing, 2D and 3D models, and CAM. Set-up covers tool holders, work holding, work offsets and proving out a program. Operation covers adjusting offsets, monitoring the cut, and stopping and restarting a cycle.

The Red Seal Occupational Standard names this block “Machines using computer numerical control (CNC) machines”. It carries 20% of the exam, about 27 of the 135 questions, split across three tasks. The share column is each task's weight within the block, as the standard publishes it.

04What the questions turn on

Canned cycles stay on until G80

A canned cycle is modal. Once G81 is active, every block with a new position repeats the cycle there with the same Z, R and F values until G80 cancels it. Axis words that are not restated keep their last value.

G43 takes H, G41 takes D

Tool length compensation is switched on by G43 with an H number. Cutter radius compensation is G41 with a D number, and it works in the plane of the contour only. Check that the H number matches the tool in the spindle.

Same error everywhere means the datum

When every feature is out by the same amount and the spacing is right, the work offset is off, not the tool or the program. Shift the work offset, and leave the proven program's coordinates alone.

Allow for the edge finder radius

When an edge finder picks up an edge, the spindle centre is still one tip radius away from it. Add or subtract half the tip diameter, in the direction of the edge, before entering the work offset.

05The other blocks

The 429A exam has eight blocks. Each has its own page of free questions:

The 429A Machinist practice exam page describes the full question bank. How these questions are written and checked: how our questions are made. Found a mistake? Tell us and we will fix it.