What is an Alphacam post-processor? Producing NC code for your machine

A post-processor (post for short) is the translator file that turns the toolpath Alphacam produces into the NC code a specific machine controller understands. The same drawing and operations come out as one file for Biesse, another for Homag, another for a local router; the post makes the difference. A wrong post means the machine either does not run or runs wrongly — the most expensive kind of CNC error. This article explains what a post does, how it is chosen and how it is tested.

What the post does

Alphacam keeps the toolpath in a machine-independent internal form: coordinates, depths, tool numbers, speeds. The post takes that and:

• Writes the program header and footer (units, plane, absolute/incremental, safe height, spindle on/off, vacuum on/off).
• Issues the tool change in the controller's command (M6 T3, or an operation block on Biesse/Homag).
• Translates moves to G-code (G0/G1/G2/G3) or the builder's macro language (WoodWOP .mpr, Xilog .xxl/.pgm, Biesse .cix/.bpp).
• Recognises drilling cycles (G81/G83 or the builder's drill block) and multi-spindle drill groups.
• Manages zero point, mirror, rotation and multi-station tables.

Controllers and dialects

Even within one brand, the controller software version affects the post; think "post for WoodWOP 7", not "post for Homag".

Where posts come from, who writes them

Alphacam ships with posts for common controllers; the post specific to your machine is installed or edited by the Alphacam reseller — writing a post needs controller knowledge and is the reseller's job. Post files live in the post folder under LICOMDIR (path varies by release); include them in your backups. When buying a new machine, ask the builder "is there an Alphacam post"; most local builders ship with Fanuc/Osai-compatible posts.

Testing a post, in order

1. Simulation: simulate the toolpath in Alphacam; this tests the toolpath, not the post, but it is the first filter.
2. Read the NC file: header (G21 mm, G90 absolute, safe Z), tool call, first move. A meaningless line means a wrong post.
3. Dry run: no board, Z at safe height, one part; watch the moves.
4. One part on scrap board: through cut + one hole; measure. If you drew 600 × 400, you must get 600 × 400.
5. Program with a tool change: two different tools; confirm the change uses the right command.
6. Drill cycle and multi-spindle: a System 32 row; check the drill group is recognised.

Common errors

• Units: inch post with a mm drawing — part 25× too small. Check G21/G20 in the header.
• Zero point: drawing origin and machine zero in different corners; the part runs off the table. Mirror/offset setting in the post.
• Safe Z: if the post default is 5 mm, clamps/vacuum pods get hit; set 30–50 mm.
• Tool number ≠ magazine: the cutter you called T3 in Alphacam sits in pocket 5 on the machine. Map tool library to magazine list.
• Direction and compensation: if the post enables cutter radius compensation (G41/G42), compensation must be off in Alphacam, or it is applied twice.
• Cutting direction: contours reversed after nesting go to the post reversed; bulk-fix with Reverse Direction (GMacros).

How posts relate to add-ins

GMacros macros and add-ins do not touch the post: they write to the Alphacam drawing (layers and geometry), Auto Style assigns the operation (Alphacam Auto Style setup: automatic machining by layer name), your post produces the NC. That is why they "run on every CNC router" — the condition is that your machine has an Alphacam post. For remote help with installation and post/Auto Style mapping: contact.