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.
Tool geometry
Cutter diameter and compensation in a CNC preview
The programmed line usually represents a tool-center path, not the finished wall by itself. To predict removed material, apply the cutter radius once and on the correct side of the geometry.
Diameter is the complete cutting width
A 9 mm cutter removes a 9 mm wide strip when its center follows a straight line. The radius is 4.5 mm, so removal extends 4.5 mm to each side. Applying 9 mm to both sides would incorrectly display an 18 mm channel.
Tool numbers do not guarantee diameters. T9 can mean tool position 9, not a 9 mm cutter. If a machine stores its tool table separately, the program may contain only the number and the viewer must request or default the physical diameter.
Centerline mode follows the programmed path
In centerline mode, the selected cutter is swept directly around the coordinates in the file. This is suitable when CAM has already offset the path, for engraving centerlines and for files that intentionally define the cutter center. It is also the safest neutral interpretation when compensation information is absent.
Compare the colored line with the resulting walls. On a straight channel, both edges should remain half the cutter diameter away from the line. Curves should remain smooth and use the same radius.
Inside and outside modes preserve different geometry
An outer profile normally keeps the finished part inside the contour, so the tool center runs outside the intended edge. An internal opening normally keeps the surrounding panel and moves the cutter toward the opening. The correct mathematical side also depends on whether the contour runs clockwise or counterclockwise.
Compensation commands such as G41 and G42 describe left or right relative to travel. They are not universal synonyms for inside and outside. A preview must combine the command with contour direction before deciding which material remains.
The outer stock boundary needs special treatment
If a path defines the final outside shape, removing material on the wrong side shrinks the part or creates a false frame. For a rectangular stock with notches, the completed boundary should follow every notch and return to its start. The cutter sweep may extend outside the stock, but only material inside the original panel can be removed.
A closed internal loop is different. One pass around that loop cuts a channel around its boundary; it does not prove that the enclosed area was pocketed. Interior material should disappear only when clearing passes actually cross it.
Assign multi-tool paths before judging the result
Multi-tool files may rough with a large cutter and clean corners with a smaller cutter. Each colored tool group needs its own diameter. Applying both diameters sequentially to every path exaggerates removal; each tool should affect only the path assigned to that tool number or color.
- Confirm diameter, not tool number
- Apply radius only once
- Check contour direction
- Protect the outer finished edge
- Keep uncleared interiors solid
- Assign each tool to its own paths
Worked example: preserving a rectangular part
A clockwise path describes the finished boundary of a 400 by 200 mm rectangle and uses a 10 mm cutter. To retain the requested part, the cutter center must run 5 mm outside the boundary. Running it 5 mm inside would remove 10 mm from both overall dimensions and produce a 390 by 190 mm result.
Internal geometry reverses the manufacturing objective: the operator normally wants to preserve the wall outside a pocket. Contour direction, G41 or G42 state and the post processor convention determine the proper side. The outermost stock outline deserves separate handling because it may be a stock declaration rather than an actual cutting command.