CAM SIMULATORCAM simulator (try CAM in your browser)
Define the shape in CAD, choose the tools and how to cut in CAM, and the toolpath is drawn, a 3D stock is cut away, and finally an NC program comes out. You can follow everything a CAM system does, start to finish, right in your browser. No installation or sign-up needed.
Change the numbers,
press “▶ Cut”
and see!
1
2
3
4
?How to use
- Choose a scene: four scenes — 2.5D pocket, 3D surface, 3+2 indexing and simultaneous 5-axis. Switch between them with the tabs above.
- CAD: define the shape: change the outline, pocket and hole dimensions, the height of the hill, the slope angle or the dome radius, and the shape and toolpath are rebuilt on the spot.
- CAM: choose how to cut: for each operation, choose the tool diameter, spindle speed, feed, stepover, depth of cut and cutting strategy. Operations that are unchecked are skipped.
- Simulation: press “▶ Cut” and the tool follows the path while the stock is cut away. The colors are on size (green), stock left (yellow) and gouge (red). Drag to rotate and use the wheel to zoom.
- Post: from the same toolpath, it generates NC programs in two dialects, FANUC-style and HEIDENHAIN. You can copy and save them.
!8 things to try
1. A tool larger than the corner radius
In the 2.5D scene, set the pocket corner radius to 3 mm and keep the pocket tool at φ8. The tool radius of 4 mm does not fit into the corners, so yellow stock left appears in all four. As a rule, make the corner radius slightly larger than the tool radius.
2. Stepover larger than the tool diameter
Set the pocket stepover to 10 mm (with a φ8 tool) and uncut ridges are left between the passes.
3. Compare zigzag, contour and trochoidal
Switch the pocket strategy among the three and compare the “machining time” below and the shape of the toolpath. Trochoidal draws small loops and removes material bit by bit, so the path gets longer, but the load on the tool (the engagement) is small, and in practice you raise the feed.
4. Use G83 for deep holes
Set the hole depth to 25 mm and the cycle to G81, and a warning appears. Switch to G83 and you can see the drill retract again and again to clear the chips.
5. Cusp height
In 3D surface finishing, change the pitch from 0.3 to 2 mm. You can see the ridges (cusps) left between the passes, and their height is shown in the note. Halving the pitch reduces the height to about a quarter and doubles the time.
6. See 3+2 from the machine’s side
In the 3+2 indexing scene, press “View from machine,” and the table tilts so that the slope becomes horizontal, and the tool, still vertical, cuts with the same motion as in 2.5D. G68.2 in the NC program (PLANE SPATIAL on HEIDENHAIN) is the command that creates the coordinates of this tilted plane.
7. How a ball end mill is used in 3-axis and 5-axis
In simultaneous 5-axis, set the tool axis to “3-axis,” and at the top you end up cutting with the ball tip (surface speed 0), and a warning appears. Go back to “5-axis” and change the lead angle from 0 to 30°, and the tool diameter at the point being cut (the effective cutting diameter) and the cutting speed change.
8. The limit of the rotary axes
In simultaneous 5-axis, set the “machine tilt limit” to 30°, and in the lower part of the dome the tool can no longer be tilted far enough, and the range of effective cutting diameter widens. On a real machine, too, the range of motion of the rotary axes determines which tool orientations you can use.
⌗What is inside this simulator, and its limits
- Material removal uses a Z-map: the stock is divided into a 0.5 mm grid, and each cell holds only its height as seen from above. Every time the tool (a cylinder, a ball or a cone tip) passes, the height of each cell is lowered to the lowest point of the tool. Surfaces that cannot be seen from above (downward-facing surfaces, undercuts) cannot be represented. The verification functions of most CAM systems calculate with a finer grid or with solids.
- All toolpaths are short straight segments: real CAM also uses arcs (G02, G03), splines and feeds that vary with the cutting load. Machining time is an estimate calculated as length ÷ feed with a 20 m/min rapid, and acceleration and deceleration are not included.
- Rotary axes in 5-axis: A and C are calculated from the tool axis direction, assuming a machine with an A axis (about X) and a C axis (about Z) on the table side. The direction of rotation (sign) and the zero position of C differ from machine to machine.
- Post: the FANUC-style program is an example that uses G43.4 (tool center point control), G68.2 (tilted-plane coordinates), G83 and so on, and the HEIDENHAIN one uses M128, PLANE SPATIAL and CYCL DEF 200. Make the NC program for a real machine with the post-processor for that machine, and check it against the machine builder’s manual.
- Warnings: it checks corner radius against tool radius, stepover, flute length against depth, collisions in rapid moves, holder collisions (vertical tools only), deep holes and surface speed at the tip.
Other CAD/CAM pages
CAD/CAM basics
The differences between CAD, CAM, and CAE, the 8 steps of the CAM workflow, types of CAM, and 35 terms.
?CAM finder
Pick your machine, part shape, rotary axes, current CAD and more to see the tier you need and CAM confirmed to support it (no ranking).
ATerms & learning path
97 terms in four levels: Beginner, Intermediate, Advanced, Applied. Plain explanations, what matters on the shop floor, common misconceptions, and a learning path for each level.
▲Axes & licenses
Tiers of 2.5D, 3D, 3+2, and simultaneous 5-axis, and whether you can add them later. Three patterns for which tier 3+2 sits in, by maker. A comparison table of 23 products.
⌂Machine builders × CAM
Partner CAM systems, certified post-processors, machine models, and in-house conversational programming and digital twins for 22 machine tool builders. How NC code differs by control.
▣CAM by machine type
12 fields including 5-face machines, simultaneous 5-axis, molds, mill-turn, Swiss-type, wire EDM, gears, and tool grinding. Dedicated CAM and the strength of the evidence.
◍Japan and the world
The global CAM market is about $3.1 billion (2025). Rankings that change with the yardstick, regional circumstances, Japan’s homegrown CAM, China, and a consolidation timeline.
≋Toolpath types
Contour, pocket, hole, high-efficiency roughing, trochoidal; waterline, raster, surface-following, pencil, rest machining. Includes calculators for trochoidal slot milling and an initial depth-of-cut guide.
▤CAD/CAM makers & products guide
57 products in 9 use-case groups. A map of groups (parent companies), CAM that runs inside CAD, strengths, industries, AI features, and Japanese contacts.
⇄Data formats
What STEP (AP203, AP214, AP242), IGES, Parasolid, ACIS, DXF, DWG, STL, and 3MF carry. Problems that occur in exchange.
⌖Coordinate systems, post, DNC
Work coordinate system G54, stock and tool library, the 4 stages of simulation, post-processor, DNC operation, and a checklist of common mistakes.
⟲5-axis machining
The difference between 3+2 and simultaneous 5-axis, machine configurations, NC functions such as tool center point control, calibration, common mistakes, and 5-axis calculations.