Bug Report: Fusion 360 Post Processor Issues with G68.2 Tilted Work Plane for HNC-848Di Control

[pavel.lagunv]

Hello Autodesk Team,

I am reporting critical issues with Fusion 360 post processor when using G68.2 (Tilted Work Plane) for 3+2 multi-axis machining on HNC-848Di CNC control.

**Machine:** IRON MAC IMU-5X 400 PRO (5-axis machining center)

**CNC Control:** Huazhong HNC-848Di

**Post Processor:** rs274 multi-axis.cps (Generic RS-274D Multi-axis)

**Fusion 360 Version:** 2026 (current)

## Problems

1. **Drilling cycles (G81/G83) are expanded to linear moves (G0/G1)** at the CAM level before post processor is called. The `onCyclePoint()` function is never called, preventing the post processor from outputting drilling cycles.

2. **Incorrect command sequence:**

   - G69 (cancel tilted plane) outputs BEFORE the operation instead of AFTER

   - G43.4 (TCP) outputs AFTER G69 instead of BEFORE G68.2

   - G53.1 outputs without feedrate (should include F3000 parameter)

   - Machine-specific commands are missing (M61 M63, M51 M53, G05.1 Q0 for HNC controls)

## Impact

Programs generated by Fusion 360 execute drilling operations in the wrong coordinate system, resulting in incorrect part geometry or potential machine crashes.

## Expected Sequence (per HNC-848Di requirements):

```gcode

M61 M63                           ← Unlock rotary axes

G0 A-90. C270.                    ← Position rotary axes

G43.4 H1                          ← Enable TCP BEFORE G68.2 ⚠️

G68.2 X0 Y0 Z0 I90. J90. K180.   ← Set tilted work plane

G53.1 F3000                       ← Turn machine (with feedrate) ⚠️

M51 M53                           ← Machine mode

G05.1 Q0                          ← High-speed mode

G0 X0. Y35.                       ← Approach point

G98 G81 Z64. R71. F20.            ← Drilling cycle ⚠️

G80                               ← Cancel cycle

G69                               ← Cancel plane AFTER operation ⚠️

G49                               ← Cancel TCP

```

## Actual Sequence (Fusion 360 output):

```gcode

G0 A-45. C15.                     ← Position rotary axes

M8                                ← Coolant on

G68.2 X0 Y0 Z0 I-165. J45. K180. ← Set tilted work plane

G53.1                             ← Turn machine (NO feedrate) ❌

G0 X-0.001 Y35.753               ← Approach point

G69                               ← Cancel plane BEFORE operation ❌

G43.4 H1                          ← Enable TCP AFTER G69 ❌

G0 X-30.287 Y113.027 Z66.452    

G1 X-11.464 Y42.779 Z-6.274 F40  ← Linear moves instead of cycle ❌

```

**Critical consequence:** The drilling operation executes in the base coordinate system instead of the tilted work plane, resulting in holes drilled in wrong locations and orientations.

## Comparison with SolidCAM

SolidCAM correctly generates the proper sequence with drilling cycles (G81/G83) in tilted work plane operations. This proves the correct sequence is technically feasible and industry-standard.

## Investigation

I added debug comments to the post processor to track function calls:

- `onCyclePoint()` is **never called** for drilling operations with G68.2

- `onLinear()` is **not called** for the expanded linear moves

- Fusion 360 outputs G0/G1 commands directly, bypassing post processor cycle handling

**Conclusion:** Drilling cycle expansion happens at the CAM level before post processor execution. The post processor cannot prevent this.

## Current Workaround

I created a custom HNC post processor with 500+ lines of modifications to fix the command sequence issues. However, I cannot fix the drilling cycle expansion problem as it happens before the post processor is called.

## Test Files Available

I have test files available for verification:

- `1001.nc` - Fusion 360 output with custom HNC post (correct sequence, but cycles still expanded)

- `1002.nc` - Fusion 360 output with standard post (incorrect sequence)

- `ST1.NC` - SolidCAM output (correct reference from working machine)

- `rs274 multi-axis HNC.cps` - Custom post processor with all fixes

I can provide these files and detailed bug report document upon request.

## Request

Please prioritize this bug fix as it affects **multi-axis drilling operations**, a core CAM functionality. The current behavior makes Fusion 360 unsuitable for production use with HNC-848Di and similar controls without extensive post processor customization.

**Affected users:**

- Users with HNC CNC controls (Huazhong HNC-848Di and similar)

- Users with Fanuc controls requiring strict G68.2 sequence

- Users requiring drilling cycles in 3+2 operations (aerospace, mold making, die making)

- Users migrating from SolidCAM, Mastercam, PowerMill to Fusion 360

## Contact

I am available for:

- Providing test files

- Testing beta fixes on IRON MAC IMU-5X 400 PRO machine

- Sharing custom post processor code

- Video demonstration of the issue

- Remote session to demonstrate on actual machine

Thank you for your attention to this critical issue.

Best regards

```

1002.nc

ST1.NC

Fusion360_Bug_Report_HNC_848Di.txt