Machine Posts

Pick the right controller

RotatoCAM writes a G-code file for your controller. Choosing the wrong entry in the Controller dropdown is the most common reason a rotary job refuses to post. This page covers which one to pick, and how to add a machine-specific post without waiting for a new release.

Genmitsu with a rotary axis

If you have a Genmitsu 4040-PRO or 3030 PROVer MAX with the 4th-axis rotary kit and you try to post a rotary or 3+1 job with grbl selected, RotatoCAM stops you with:

GRBL (3018/3040) is 3-axis only, but this toolpath has rotary moves.

That message is correct for a 3018, and wrong for your machine.
Genmitsu machines with the rotary kit do not run stock GRBL. Their controller is a 4-axis build, and the rotary axis is A. The grbl entry assumes a three-axis board and refuses anything with rotary motion in it.

Option 1 — use grblHAL, nothing to install

Works immediately with the copy you already have.

Open RotatoCAM.
Scroll the left-hand settings column down to the Post / Machine box.
Set Controller to grblhal instead of grbl.
Generate as normal. The output uses the A axis your controller expects.

Option 2 — install the Genmitsu post

Adds a clearly-labelled genmitsu entry to the dropdown, so you never have to remember that grblHAL is the right pick. One file, no reinstall.

Download genmitsu.py All posts

Close RotatoCAM if it is running.
Press Windows + R, type this and press Enter:
```
%USERPROFILE%\.rotatocam\posts
```
A folder opens. If it does not exist, open %USERPROFILE% instead, create a folder named .rotatocam (keep the leading dot), and inside it create one named posts.
Copy genmitsu.py into that folder. The finished path looks like:
```
C:\Users\<you>\.rotatocam\posts\genmitsu.py
```
Start RotatoCAM.
Post / Machine → Controller now lists genmitsu (custom). Pick it.
Generate your program.

Why a separate post? It pins the rotary axis letter to A, which is what Genmitsu firmware actually drives, and ignores the job's rotary-letter setting. A job configured for a C axis would otherwise emit words the machine cannot act on, and the rotary would stand still while the cutter moved.

HolzProfi CNC6090 on the HC-204A

Pick the hc204a controller, and in Machine setup set Rotary runs along to Y, because on this machine the chuck points down the Y axis rather than X. There is a HolzProfi CNC6090 (HC-204A) machine preset that sets both for you. Travels are not in the preset on purpose: the HC-204A manual describes the control, not the machine it is bolted to, so measure your own and type them in.

This post is built from the HC-204A manual rather than guessed at, and the manual is unusually strict about what it accepts. Its complete G list is G00 G01 G02 G03 G04 G17 G18 G19 G28 G43.4 G49 G50.1 G51.1 G53 G54-G59 G90 G91, and its M list is M03 M04 M05 M08 M09 M12 M13 M30 M34 M35 M60 M61. Three things follow from what is missing from those lists.

No G93 and no G94, so there is no feed-mode word to send. Rotary feeds are converted into ordinary per-minute feeds rather than relabelled, the same approach the AtomStack post takes. The cost is inherent: cutter-contact speed then varies with radius.
No G20 and no G21, so the post is metric-only and will refuse an inch job rather than emit a units word the control does not know.
No M06 and no M00, so there is no documented way to pause a running program for a tool change. Rather than emit a pause that might not pause, the post refuses multi-operation programs. Export each operation as its own file and change tools at the pendant.

Yes, it does simultaneous four-axis. The manual's parameter table has a Speed ratio of rotating shaft setting described as applying "in 4-axis linkage", with an HC-204A default of 2, and the model list calls it a "single-head 4-axis handheld control system". Be aware of what that parameter means for you, though: the machine scales rotary speed by a number RotatoCAM cannot see, so the real rotary rate is the emitted feed times a setting on your control.

Experimental, and one thing to check on your own Fusion post. No RotatoCAM program has been cut on an HC-204A yet, so air-cut the first one. Separately: the widely shared Fusion post for this machine writes A0 onto every ordinary three-axis move. If the part is indexed to A90, the next plain move commands the rotary back to zero, possibly with the cutter down. RotatoCAM only ever writes a rotary word on a block that genuinely has a rotary position, so it cannot do that, but it is worth knowing if you are running the Fusion post today.

What we do not know yet

Three things the HC-204A manual does not answer. None of them stops you trying the post, and all three are things you can settle in ten minutes at the machine. If you find out, please say so and the built-in post gets fixed for the next owner.

Does A past 360 keep turning, or wrap? A continuous finish spiral emits A450, A720, A1080 and so on, and RotatoCAM deliberately never wraps them. Jog to G90 G0 A370 and watch: if the rotary carries on the same way, you are fine. If it unwinds to 10 degrees, tell us, because then a spiral needs different handling.
How does it time a block when A moves with XYZ? The feed conversion assumes the control counts rotary degrees as if they were millimetres, which is what grbl does, because nothing better is documented. If your rotary moves run obviously fast or slow against the linear ones, this assumption is the reason.
Is G04's P word seconds or milliseconds? The manual lists the code but not its timebase. The spindle warm-up dwell is emitted as G4 P<seconds>, so on a millisecond control a 2 second warm-up quietly becomes 2 milliseconds. That fails safe, but set the dwell to 0 in Post settings if you would rather it were not in the file.

Using RotatoCAM 0.69.2.223.13? The HC-204A post is built into 0.69.2.223.14 and later. On .13 it is not, so download the drop-in below, put it in %USERPROFILE%\.rotatocam\posts and restart. It produces byte-identical G-code to the built-in. You still need .13 or later for the Rotary runs along setting.

Download hc204a.py View source

Which controller do I pick?

Your machine	Controller
Genmitsu 4040-PRO / 3030 PROVer MAX + rotary kit	`genmitsu` or grblhal
3018 / 3040 3-axis only	`grbl`
grblHAL board 4-axis	`grblhal`
AtomStack C4 Pro	`atomstack` experimental
HolzProfi CNC6090 HC-204A, rotary along Y	`hc204a` experimental
LinuxCNC	`linuxcnc`
Mach3 / Mach4	`mach3` / `mach4`
Centroid Acorn / Oak	`centroid`
MASSO G2 / G3	`masso` experimental

Writing your own post

Anything you drop in %USERPROFILE%\.rotatocam\posts appears in the dropdown tagged (custom). The folder contains a README.txt with a minimal working example. A post that errors is skipped and logged; it will not stop the app from starting.

Only add posts you trust. Files in that folder are executed as code when RotatoCAM starts.

Before you cut

Air-cut every new post first. Run the program with the tool clear of the work, or with a marker in the collet, and watch that the rotary turns the way you expect. G-code is only ever a suggestion, and you are the last line of defence.

3+1 indexed work is ordinary G-code and low risk. Fully simultaneous 4-axis output on a Genmitsu has not yet been confirmed on a machine by anyone, so treat the first one as a dry run and tell us how it went.