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.
Toolpath fundamentals
How to read a CNC toolpath before the first cut
A toolpath drawing shows where the programmed tool center moves. A solid simulation goes one step further and estimates the material removed around that centerline. Understanding the difference makes it easier to spot an incorrect diameter, depth or compensation setting.
Tool diameter is the full cutting width
Selecting a 9 mm cutter means the swept path is 9 mm wide, with 4.5 mm extending to each side of the tool centerline. It does not create an 18 mm channel. If a file identifies only a tool number, the physical diameter may live in the CNC machine's separate tool database. In that case the viewer cannot safely infer the diameter from the number alone.
Z values and cutting depth
G-code commonly uses the top face as Z zero, so a move to Z-6 removes 6 mm from the top. Woodworking formats can also measure Z from the panel bottom. On an 18 mm panel, a cutting level of Z12 then represents a 6 mm top channel. Safe approach and retract heights must be excluded; otherwise a viewer can incorrectly display a shallow channel as a complete through-cut.
Centerline, inside and outside compensation
With centerline processing, the cutter center follows the programmed geometry. Inside and outside modes shift the swept area relative to the contour. For an outer profile, the cutter normally runs outside the finished boundary so the part keeps its intended dimensions. For an internal pocket, the correct side depends on contour direction and the compensation command written by the post processor.
When compensation is absent or ambiguous, compare the toolpath overlay with the solid model. The finished edge should remain on the expected side of the colored centerline.
Drilling, channels and surface machining
Vertical holes
Check diameter, top or bottom surface, depth and whether the cycle passes through the stock.
Horizontal holes
Confirm the entry edge, direction, center height and depth. A dark mark without a visible bore usually indicates an incomplete side-hole interpretation.
Open channels
The remaining material around a channel should stay solid. Only the area swept by the selected cutter is removed.
Closed contours
A closed loop is not automatically a pocket. The program must contain the passes that clear its interior, or the center remains solid.
Simulation density and accuracy
Density controls the resolution of the calculated surface. A higher setting makes curved edges and small cutters look smoother but uses more memory and processing time. It should not change the programmed dimensions. Start with Medium for inspection, then use High or Ultra when a small feature needs a closer visual check.
A practical inspection sequence
- Load the file and verify stock dimensions.
- Review tool colors and assign missing cutter diameters.
- Compare the toolpath overlay with the removed solid volume.
- Switch between top, front, back, left, right and bottom views.
- Open statistics and confirm every hole and channel operation.
- Generate the technical drawing for dimensions and relative positions.
Worked example: a 9 mm cutter on an 18 mm panel
A centerline runs from X20 Y40 to X180 Y40 at Z-6. With a 9 mm flat cutter, the removed channel is 9 mm wide and 6 mm deep: its edges lie 4.5 mm on either side of Y40. The untouched 12 mm below the channel must remain solid. Selecting Outside compensation shifts the cutter center relative to a contour; it does not double the cutter to 18 mm.
Now add a second 3 mm cutter assigned to a different colored path at Z-8. The second operation begins from the material left by the first and removes only places its own 3 mm footprint reaches. It should not globally shrink the first channel or clean areas that have no second-tool path.