Why the SimCam CNC output doesn’t look like you want (and how to fix it)

Modified on Mon, 29 Sep at 3:33 AM

SimCam is designed to speed up toolpath creation. It generates generic, FANUC‑style G‑code that works as a starting point. Every shop and controller has its own conventions, so you’ll usually need light edits (post‑style tweaks) before running on a real machine.

Bottom line: SimCam assists the programmer; it doesn’t replace one. You remain responsible for verifying code before cutting.

Common reasons the code doesn’t “look right”

Different controller dialects: Haas vs. FANUC vs. Siemens vs. Okuma, etc.
Header/ footer style: program numbers (O1234), G17/G40/G49/G80/G90 preamble, M30 vs M2, comment style (…) vs ;.
Units/formatting: mm vs inch, decimals/leading zeros, feed in mm/min vs inch/min.
Tool/coolant calls: Txx M06, M08/M09, spindle syntax Sxxxx M03/M04.
Work offsets: G54–G59 vs. G92 or local shifts.
Arcs: center format I J K vs radius R, arc plane (G17/G18/G19).
Canned cycles: drilling/boring (G81–G89), peck/ream/tap variations.
Subprograms / repeats: M98 Pxxxx L vs explicit repeats.

Quick wins: make the output match your shop

Decide your house style (once):
- Header: O####, G17 G40 G49 G80 G90, units (G21/G20), work offset (G54).
- Footer: spindle/ coolant off, retract, M30.
- Comment style, decimal precision, feed/spindle formatting.
Set SimCam’s output preferences (decimals, format, leading and ending blocks, etc.).
- Try different settings and test the output.
Create a reusable header/footer template. Paste this at the top/bottom of every program (or set the Leading and Ending blocks to merge automatically):
```
(JOB: <name>) O1000 G17 G21 G40 G49 G80 G90 G54 (TOOL 1: <desc>) T1 M06 S1200 M03 M08
```
…
```
M09 G28 G91 Z0 G90 M30
```
Map codes with quick find/replace rules. Keep a small table you can apply in your editor:
From To Notes
; ( ) Convert to parentheses comments
M2 M30 Shop standard end code
R… in arcs I J If your control requires center format
G55 G54 If you standardize on G54
Standardize tools and offsets. Ensure your tool numbers (T01/T1) and length/diameter comp (G43 Hxx, G41/G42 Dxx) match what’s set on the machine.
Simulate and prove out.
- Run inside the simulator first.
- On the machine: graphics/ dry run, single‑block, feed‑hold ready.

From	To	Notes
`;`	`( )`	Convert to parentheses comments
`M2`	`M30`	Shop standard end code
`R…` in arcs	`I J`	If your control requires center format
`G55`	`G54`	If you standardize on G54

“Will SimCam ever output my exact machine’s code?”

Not perfectly for every brand/option combination. Controllers vary widely, and shops prefer different preambles, cycles, and macros. SimCam aims to produce solid, readable “FANUC‑like” output that you tailor for your environment.

Safety & responsibility

You must verify that the program is correct and safe for your machine before cutting. Check units, work offsets, tool lengths, and any canned cycles outside the simulator environment.