A practical CNC preview verification checklist

1. Confirm the file and stock

Check the filename, units, length, width and thickness before judging any machining detail. A millimeter program interpreted as inches is obvious, but a 15 mm panel interpreted as 18 mm can remain visually plausible while every bottom operation is wrong.

• Correct file and revision
• Millimeter or inch units
• Stock length and width
• Physical panel thickness

2. Match tools to colored paths

Review every tool group separately. Confirm that the displayed diameter is a physical cutter diameter rather than a tool number. For files with missing tool tables, assign the known diameter and check whether a second tool performs cleanup or a genuinely separate path.

Turn the solid result off briefly and inspect the raw paths. Unexpected long diagonals often indicate positioning moves that were classified as cutting. A color change should correspond to a tool change or another meaningful group in the source.

3. Compare toolpaths with removed volume

Turn both the toolpath and 3D result on. Every cutting line should have a corresponding swept area, and every removed area should be explained by a cutting path or explicit operation. Small islands left between dense parallel passes can indicate insufficient surface resolution, while large unexplained gaps usually indicate a parsing or tool assignment problem.

Increase density only after dimensions and tools are correct. Higher density smooths small curves and narrow passes; it must not change the intended width or depth.

4. Inspect holes and channels from several views

Use top and bottom views for vertical drilling. Use front, back, left and right views for horizontal holes. Confirm the entry face, center position, diameter, depth and whether the feature passes through the stock. A side hole should remove a cylindrical bore, not only darken the entry surface.

For channels, measure the swept width against the assigned cutter. For pockets, confirm that clearing passes cover the interior. A closed path alone should not erase all material inside it.

5. Check contours, notches and remaining material

Follow the outer finished boundary around the entire panel. Notches and corner cutouts should appear both in the solid result and the technical drawing. Cutter compensation should preserve the intended part side of that boundary.

Look for thin walls, isolated columns and covered openings. If a path crosses those areas at cutting depth, the material should not remain. If no cutter passes through an enclosed area, that area should stay solid even when its boundary is closed.

6. Finish with statistics and technical drawing

Compare the operation count with the program. Repeated setup records should not create duplicate holes, but operations on different faces or with different diameters must remain separate. In the technical drawing, verify overall size first, then reveal detailed measurements and select individual features when labels become crowded.

1. Confirm overall dimensions and coordinate origin.
2. Check hole positions from stable panel edges.
3. Measure notch opening, depth and remaining outside shape.
4. Compare channel endpoints, width and cutting depth.
5. Return to the source program for every unexplained feature.

Worked review: diagnose a suspicious closed area

A closed blue contour appears around a central region, but the 3D model leaves the center solid. First check whether the program contains only one perimeter pass or also contains clearing passes. A closed line by itself cuts a channel around the region; it does not prove that the interior was pocketed.

Next confirm the cutter assigned to that color and compare its radius with the visible channel. Hide the grid, inspect from top and side views, and use statistics to verify the operation depth. Finally open the technical drawing: if it shows only the contour centerline, the solid center is expected. If dense clearing paths cross the area but material remains, the removal calculation needs correction.