MET
THFree trial

Manual / CAM

CAM overview

Create 2.5D / 3D milling and turning toolpaths from a part, simulate the cut, and generate G-code.

Edition: Premium

What it does

The CAM tab creates toolpaths for 3-axis CNC mills and lathes from a part in Part Design or from a STEP/IGES/STL file. It simulates material removal with collision checking, then generates G-code and a setup sheet. Jobs are saved as .metcam.

CAM tab with a four-operation name plate job open
CAM tab with a four-operation name plate job open

Parts of the window

Part Description
CAM Manager (left) Setup 1 (mill/lathe): Geometry, Stock, Clearances, Frames, Tools, Operations, Machine, Output
Ribbon Model, Machining, 3D Milling, Simulation, Output
Status badge (top right) Mill job / Lathe job (sample jobs: Demo (read-only) - use Save As)
✕ Close CAM Closes the CAM job (asks to save) and clears the toolpaths
Properties (right) Settings for whatever is selected in the CAM Manager

Model tab: Job, Part, Setup, Tools, Learn
Model tab: Job, Part, Setup, Tools, Learn

Machining tab: Turning (lathe) / 2.5D Milling (mill)
Machining tab: Turning (lathe) / 2.5D Milling (mill)

3D Milling tab: 3D Rough, 3D Finish, Tactics
3D Milling tab: 3D Rough, 3D Finish, Tactics

Simulation tab: Simulate, Ortho, Persp
Simulation tab: Simulate, Ortho, Persp

Output tab: Post, G-code, Shop PDF
Output tab: Post, G-code, Shop PDF

Workflow

  1. New Job. Choose a Mill or Turn template.
  2. Check the Stock, Frame (WCS) and Clearances.
  3. Add tools from the Tool Library.
  4. Add operations: Face/Pocket, Profile, Drill, 3D, Turning.
  5. Simulate.
  6. Generate G-code and Shop PDF.

Note: A lathe job hides the 3D Milling tab and the 2.5D group. A mill job hides the Turning group. If the window is narrow, buttons that do not fit move into the » menu. CAM Undo/Redo use Ctrl+Z / Ctrl+Y.

Note: CAM is available only in MECHCAD Premium (and during the trial).

Try it: Mill a door name plate from start to finish

A 130 × 40 mm aluminium name plate with a recessed panel and two screw holes takes you through the whole CAM workflow, from model to G-code, in about ten minutes.

  1. In Part Design, sketch a 130 × 40 rectangle on XY starting at the origin and Extrude it 6 mm.
  2. Sketch on the top face: a 100 × 24 rectangle 15 mm from the left edge and 8 mm from the front edge, with R4 corners. Extrude Cut it 1.5 mm. Then add two Ø6 circles at X 7.5 and X 122.5 (Y 20) and Extrude Cut them Through All.
  3. Open the CAM tab › New Job › Mill Template › OK. The stock becomes 132 × 42 × 6.5 mm.
  4. Click Face, click the top face and press Enter.
  5. Click Pocket, click the floor of the recessed panel and press Enter. Top Z 6 and Floor Z 4.5 are read from the model.
  6. Click Drill, click both hole walls and press Enter. The T2 6 mm drill matches the holes.
  7. Click Profile, click a bottom outer edge of the plate and press Enter. In Properties › Levels, set Bottom / Floor Z to 0 so the plate is cut free.
  8. Click Simulate, then Play. The estimated time is about 6.8 min. Finish with Output › G-code and save name_plate.nc (FANUC_MET 3Axis post, about 240 lines).

Name plate: Face, Pocket, Drill and Profile toolpaths on the left, the simulated plate on the right
Name plate: Face, Pocket, Drill and Profile toolpaths on the left, the simulated plate on the right

Challenge: Change the Face cutter to T3 12mm 3F face mill (Properties › Tool › Cutter / insert) and Simulate again. How much shorter is the estimated time?

See also