Hello Guest it is August 12, 2020, 03:03:02 PM

Author Topic: Code wrong?? Broken tool :(  (Read 3712 times)

0 Members and 1 Guest are viewing this topic.

Offline Davek0974

*
  •  2,597 2,597
    • View Profile
    • DD Metal Products Ltd
Code wrong?? Broken tool :(
« on: September 09, 2016, 02:07:24 PM »
Ok, so yesterday i had a great run on the mill, one part, 6 tool changes, perfect result.

Tonight was a simple part - face, spot, drill 3 holes.

So, I set the ref's with my Haimer, the face cut works nicely, good finish, requests the spotting drill, drill fitted, Z drops to below the vice and then proceeds to snap my nice new bit off by ramming it into the back of said vise :( Much language and head scratching follows. I did hit the big red button but was too late to save the bit.

Ok, new bit fitted, ref'd the machine again, reset my co-ordinates, run the part again, facing cut took nothing off of course, just a whisper, spot drill requested again, fitted, this time i had my fist over the stop button, watched and yes it drops the Z way too low for the tool, stop pressed, give up for the night.

Now, had a glass of wine with me tea, and looking at the code (fusion 360 CAM) I see it is asking for a Z30 move BEFORE applying the tool offset !

Surely that is a crap error - the previous tool was shorter than the spot drill and the height it was heading for was correct for that tool of course but put the longer spot drill in and - snap.

Just so i know where to head, is this a Fusion 360CAM error, post error or just me being a twat ( I doubt it this time though )

Surely it MUST apply tool offset before commanding ANY Z axis move?
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.
Re: Code wrong?? Broken tool :(
« Reply #1 on: September 09, 2016, 02:22:40 PM »
On other CNCs the H word called tool length offset, not to T word. I see an H word after the XY moves. Just grasping here.

Offline Davek0974

*
  •  2,597 2,597
    • View Profile
    • DD Metal Products Ltd
Re: Code wrong?? Broken tool :(
« Reply #2 on: September 09, 2016, 02:34:18 PM »
This might help, its the raw code, first op works, second op fails. The placing and format of the G43 seems wrong in 2nd op??

Code: [Select]
(FACE3)
N20 M5
N25 M9
N30 T12 M6
N35 S3000 M3
N40 G54
N45 M7
N55 G0 X136. Y7.5
N60 G43 Z22.5 H12
N65 Z2.
N70 G1 Z-1. F900.
N75 X-20. F1400.
N80 Z-2.5
N85 X136.
N90 G0 Z22.5

(DRILL1)
N100 M5
N105 M9
N110 M1
N115 T3 M6
N120 S3000 M3
N125 G54
N130 M7
N135 G0 Z30.
N145 G0 X15. Y7.5
N150 G43 H3
N160 Z5.
N165 G98 G81 X15. Y7.5 Z-4.5 R-0.5 F535.
N170 X58.
N175 X101.
N180 G80
N185 Z30.

Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline Davek0974

*
  •  2,597 2,597
    • View Profile
    • DD Metal Products Ltd
Re: Code wrong?? Broken tool :(
« Reply #3 on: September 09, 2016, 02:38:52 PM »
Just read through a much larger job i did yesterday and the G43 line is ALWAYS G43 Z30.0 Hxx

SO something is upsetting the post it seems.??
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline Stuart

*
  •  230 230
    • View Profile
Re: Code wrong?? Broken tool :(
« Reply #4 on: September 09, 2016, 03:10:36 PM »
Hi

If it helps I had the same problem with Mach 4 and fusion360

It's the z move in the g43 line

It should not be there so Mach support told me

The code should be
G43 H12
Z22.5




Its based on a tormach post with the root from a haas one

Stuart
Let me get on the iMac and I will post it

stupid forum software
change the .txt to .cps
put it in your personal post folder ( don't know where it is on windows )

« Last Edit: September 09, 2016, 03:18:02 PM by Stuart »

Offline Davek0974

*
  •  2,597 2,597
    • View Profile
    • DD Metal Products Ltd
Re: Code wrong?? Broken tool :(
« Reply #5 on: September 09, 2016, 03:16:21 PM »
So your'e saying all the other code is wrong and this one is right, but backwards?

All the posted code i have has G43 Zxx Hxx format and works ok, this one has the Z before the G43 so must be wrong?
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline Stuart

*
  •  230 230
    • View Profile
Re: Code wrong?? Broken tool :(
« Reply #6 on: September 09, 2016, 03:19:32 PM »
mine was failing after two tool changes , two was ok
ran a job today with 5 tool changes and all was OK

Stuart

Offline Stuart

*
  •  230 230
    • View Profile
Re: Code wrong?? Broken tool :(
« Reply #7 on: September 09, 2016, 03:22:49 PM »
sample code only a two too job

Offline Hood

*
  •  25,846 25,846
  • Carnoustie, Scotland
    • View Profile
Re: Code wrong?? Broken tool :(
« Reply #8 on: September 09, 2016, 03:27:44 PM »
After a tool change you should not have any Z movements until you have called the tool height offset.
Not sure whether it matters if there is a Z call on the G43H line  but my BobCAD post puts a move there and there are no probs, for example
N01 T75 M6
S1400 M3
G0 G90 G54 X26.678 Y24.157
G43 H75 Z25.4 M8
Z5.08


Hood

Offline Davek0974

*
  •  2,597 2,597
    • View Profile
    • DD Metal Products Ltd
Re: Code wrong?? Broken tool :(
« Reply #9 on: September 09, 2016, 03:28:58 PM »
Its odd, i have other code that uses the same tool and it works ok, i have messed with just about all the settings in this part and just cant make it get that line correct.
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.