BUG - drill operation

[michalzywczak]

When generating g-code from drilling operations, Fusion 360 adds something like this:
G1 F0.
which of course generates an error in the machine (feed is ZERO).

A few days ago g-code generated from the same project was fine.

Full g-code:

(1001)
(T34 D=3. CR=0. TAPER=45DEG - ZMIN=-1.9 - CHAMFER MILL)
G90 G94 G91.1 G40 G49 G17
G21
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)

(DRILL1)
M5
T34 M6
S9000 M3
G4 P1.875
G54
G0 X7.204 Y-7.091
G43 Z15. H34
G1 F0.
G0 Z5.
G98 G81 X7.204 Y-7.091 Z-1.9 R5. F600.
X21.914 Y-7.786
X21.25 Y-27.511
G80
G1 Z15. F0.

M5
M30

[seth.madore]

What machine and post processor are you using? 
Can you export and share a file?
File > Export > Save .f3d to local file, return to thread and attach the .f3d in your reply

[michalzywczak]

Thank you for sesponse.

Machine: Mach3 milling

post: "CNC Router Parts (Mach3Mill)"

Attached exported Fusion file

Can't attach generated g-kode 😕

Error from mach3: "Cannot do g1 with zero feed rateLine 13"

[lnsubscribe]

Same problem exporting using the Carbide3D processor, GRBL error;

"Feed rate has not yet been set or is undefined"

Bugs at both the beginning and end of the file where;

G1 F0
G0

Sets the feed rate to zero causing the initial issue at the start of the job and then there is another F0 at the end of the file setting feed rate to zero again so even if you fix the first bad g-code the job halts at zero feedrate at the end of the op.

[seth.madore]

That's extremely odd. Was that on that exact part you shared? 

I logged into my sons personal account and ran your file through the generic Carbide3D and Mach3 post, this is what I got for the Mach 3:

(1003)
(6666)
(T1  D=1.7 CR=0. TAPER=118DEG - ZMIN=-10. - DRILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

(DRILL1)
M5
T1 M6
S12000 M3
G54
M8
G0 X0. Y0.
G43 Z15. H1
Z5.
G98 G81 X0. Y0. Z-10. R5. F306.
G80
Z15.

M9
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

And this was the Carbide3d:

(1001)
(6666)
(T1  D=1.7 CR=0 TAPER=118deg - ZMIN=-10 - drill)
G90
G17
G21
G28 G91 Z0
G90

(Drill1)
T1 M6
S12000 M3
G54
M7
G0 X0 Y0
Z15
Z5
G1 Z-10 F306
G0 Z5
Z15
M9
G28 G91 Z0
G90
G28 G91 X0 Y0
G90
M30

There's no rogue G1 F0 to be found....

[johnswetz1982]

Is your sons a educational account? You should be getting a warning about the personal license change like poster had in his initial comment. Perhaps this license change thing has not been fully test if 2 different post are having the same error/issue.

[lnsubscribe]

I think that was Michal's part, here's mine if that's useful. I've been able to repeat this issue on several models and none of them generate a valid to GRBL drilling operation.

Op 1 Spot Drill from the attachedopens with;

%
(Op 1 Spot Drill - 4mm Spot Drill)
(Finishing)
(T9994 D=4 CR=0 TAPER=90deg - ZMIN=0 - spot drill)
G90
G17
G21
(When using Fusion 360 for Personal Use, the feedrate of rapid moves is reduced to match the feedrate of cutting moves, which can increase machining time. Unrestricted rapid moves are available with a Fusion 360 Subscription.)
G28 G91 Z0
G90

(Spot Drill)
T9994 M6
S2500 M3
G54
G0 X26 Y26
Z20
G1 F0
G0 Z10

And that's from;

V 2.0.9.009

macOS 10.15.6

The model Simple Test Paths is in the Shapeoko project if it's easier for you to grab it from cloud storage.

I've also attached a screenshot of the post process dialog box to confirm the options there.

[michalzywczak]

@seth.madore wrote:

 Was that on that exact part you shared? 

---

 No. I generated a file specifically for this post. Here is g-code I received:

(DRILLING PROBLEM)
(T1  D=1.7 CR=0. TAPER=118DEG - ZMIN=-10. - DRILL)
G90 G94 G91.1 G40 G49 G17
G21
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)

(DRILL1)
M5
T1 M6
S12000 M3
G54
M8
G0 X0. Y0.
G43 Z15. H1
G1 F0.
G0 Z5.
G98 G81 X0. Y0. Z-10. R5. F306.
G80
G1 Z15. F0.

M9
M30

[seth.madore]

Okay, now I'm seeing it. There was something going on with my sons account, so I started a new one. I too am seeing that. I will log this with the dev team and hopefully get some eyes on this soon....

[seth.madore]

I've logged this as CAM-24897 and pinged the respective developers. It's evening and the weekend, so.....it might be a bit.

[lnsubscribe]

Thanks,

Now that the issue is identified and localised I know how to manually edit both of the F0 entries to non-zero speeds so that the file will run so it's no longer stopping me building stuff.

For anyone else with the bug, open up the nc file, choose a feed rate you're happy with for the move in and out before and after the op, I just took the drill plunge speed from the file, which is "Plunge Feedrate" in your spot drill toolpath dialog box;

(Spot Drill)
T9994 M6
S2500 M3
G54
G0 X26 Y26
Z20
G1 F0
G0 Z10
Z7
G1 Z4 F100
G0 Z10

In that case it's 100, use that or a similar safe number to edit both of the F0 entries;

(Spot Drill)
T9994 M6
S2500 M3
G54
G0 X26 Y26
Z20
G1 F100
G0 Z10
Z7
G1 Z4 F100
G0 Z10

Here's the F0 at the end of the file, change that to F(your plunge speed) too;

G0 Z10
G1 Z20 F0
G28 G91 Z0
G90
G28 G91 X0 Y0
G90
M30

Should be a fairly easy hole in the test coverage for the devs to fix. Clearly there were some oversights in the regression testing for this change.

Liam

[seth.madore]

We pushed out an update today that addresses this issue in addition to a couple others that were plaguing the Personal Entitlement community. Terribly sorry for the significant inconvenience that these particular issues caused.

Issues fixed:

1) G1 F0. feedrates on drilling toolpaths.

2) Too long "rapid reduced" comment

3) Correct feedrates not being posted for plasma/laser

[markY6RWE]

 problem here. Using Mach3 PP

I am using Windows 7 though. I tried the same file on my Windows 10 machine without the G0 and G1 lines. Here is the file generated from the windows 7 machine, one time the G0 and G1 codes were on lines 20 and 21 here they are on lines 20 and 61. When i removed those lines the file ran fine.

EDIT: not G0 I t should read G1 F0. with the period after F0

[markY6RWE]

Perhaps Im not updated yet, I just ran the file on Windows 7 and had the same errors Line 18 and Line 61, Ill go in my house and generate one on my windows 10 machine in a few min.

(1001)
(MACHINE)
( VENDOR AUTODESK)
( DESCRIPTION GENERIC 3-AXIS)
(T8 D=0.033 CR=0. TAPER=118DEG - ZMIN=-0.1463 - DRILL)
G90 G94 G91.1 G40 G49 G17
G20
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)
G28 G91 Z0.
G90

(DRILL3)
M5
T8 M6
S5000 M3
G54
M8
G0 X-1.0685 Y-0.1752
G43 Z0.6 H8
G1 F0.
G0 Z0.2
G98 G81 X-1.0685 Y-0.1752 Z-0.1463 R0.2 F40.
X-0.9685
Y-0.0752
X-1.0685
Y0.0248
X-0.9685
Y0.1248
X-1.0685
Y0.2248
X-0.9685
X-0.5685 Y0.1748
X-0.4685
X-0.3685
X-0.2685
X-0.1685
X-0.0685
X0.0315
X0.1315
X0.2315
X0.3315
X0.4315
X0.5315
X0.6315
X0.7315
Y-0.1252
X0.6315
X0.5315
X0.4315
X0.3315
X0.2315
X0.1315
X0.0315
X-0.0685
X-0.1685
X-0.2685
X-0.3685
X-0.4685
X-0.5685
G80
G1 Z0.6 F0.

M9
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

[markY6RWE]

Ok Same file Generated Gcode file on Windows 10 machine , It works from Windows 10

(1001)
(MACHINE)
( VENDOR AUTODESK)
( DESCRIPTION GENERIC 3-AXIS)
(T8 D=0.033 CR=0. TAPER=118DEG - ZMIN=-0.1463 - DRILL)
G90 G94 G91.1 G40 G49 G17
G20
G28 G91 Z0.
G90

(DRILL3)
M5
T8 M6
S5000 M3
G54
M8
G0 X-1.0685 Y-0.1752
G43 Z0.6 H8
Z0.2
G98 G81 X-1.0685 Y-0.1752 Z-0.1463 R0.2 F40.
X-0.9685
Y-0.0752
X-1.0685
Y0.0248
X-0.9685
Y0.1248
X-1.0685
Y0.2248
X-0.9685
X-0.5685 Y0.1748
X-0.4685
X-0.3685
X-0.2685
X-0.1685
X-0.0685
X0.0315
X0.1315
X0.2315
X0.3315
X0.4315
X0.5315
X0.6315
X0.7315
Y-0.1252
X0.6315
X0.5315
X0.4315
X0.3315
X0.2315
X0.1315
X0.0315
X-0.0685
X-0.1685
X-0.2685
X-0.3685
X-0.4685
X-0.5685
G80
Z0.6

M9
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30