Prepared from parser behavior, machining-file examples and visual checks performed in CNC Viewer. Always confirm the result against the CAM setup and machine documentation before production.
Depth verification
How to identify CNC Z zero and cutting depth
A negative Z value does not always mean the same thing, and a positive Z value is not always a retract. Before judging a 3D preview, establish the stock thickness, reference face and cutting convention used by the post processor.
Start with the coordinate reference
Many general G-code programs place Z zero on the top face. A plunge to Z-6 then represents a 6 mm cut from the top. Woodworking systems may describe a feature from the panel bottom instead. On an 18 mm panel, a machining level at Z12 can represent the same 6 mm top cut because the remaining material below the tool is 12 mm.
Do not infer the origin from one coordinate alone. Look for stock declarations, setup comments, safe approach values, repeated drilling levels and the direction in which cutting moves enter the material.
Separate positioning moves from cutting moves
A program can move rapidly above the stock, feed down to a cutting level, follow a contour and retract. Only the part of that sequence in contact with the material should remove stock. Treating every Z change as a cut creates walls, spikes or full-depth slots that the machine never produces.
Feed mode is useful evidence but not a complete rule. Some post processors use a high feed move instead of a rapid command. A reliable check combines motion type, feed rate, spindle state, neighboring Z values and whether the XY path continues at the same cutting level.
Blind cuts and through-cuts need different checks
A blind pocket must leave a measurable floor. If an 18 mm panel is cut 7 mm from the top, approximately 11 mm remains. A through-cut normally reaches the opposite face and may continue slightly beyond it into a spoilboard allowance. The preview should clamp removal to the stock; the extra programmed depth must not create geometry below the panel.
For a hole, compare the declared depth with the stock thickness and entry face. A 20 mm drilling depth through an 18 mm panel is plausible. The same value for a horizontal edge hole is not comparable until its entry edge and drilling direction are known.
Positive-Z relief programs require context
Some carving and relief files store surface heights as positive Z values. In that convention, the highest programmed surface can align with the stock top while lower values indicate deeper removal. A viewer may need the physical stock height before it can convert those heights into machining depth.
A fast XY move at a high feed can also be a positioning move even when it uses G1. Confirm the expected rapid threshold and stock height when the file does not include reliable setup metadata.
A practical Z verification checklist
- Confirm physical stock thickness
- Identify the top or bottom reference
- Find safe approach and retract levels
- Compare feed moves with spindle state
- Check the remaining floor thickness
- Inspect through-cuts from the bottom
Worked example: approach, cut and retract
On an 18 mm panel with top-face zero, a sequence moves rapidly to Z5, feeds to Z-4, travels across the panel and returns to Z5. Only the horizontal movement at Z-4 cuts a 4 mm-deep channel. The two vertical transitions may show machine motion, but the segment above Z0 must not remove stock or increase the reported depth.
If the same post expresses height from the panel bottom, the cutting level may instead be Z14 because 18 - 14 = 4 mm. This conversion is valid only after the reference convention is established from file headers, format rules or consistent operation data. Choosing the numerically smallest Z value without that context can invert the complete model.