Doosan DNM4500 G17 issue

TSmcam · May 27, 2025, 06:36 PM

I've got a customer running a Doosan with a Fanuc 32i control.

They ran a program that when from a drilling toolpath ending with G80, then a return to home with an optional stop. The next toolpath was a chamfering toolpath, with arc commands, in the XY plane.

The drilling toolpath was fine, and then it toolchanged, and when cutting the chamfer, it did a weird arc move, and gouged the part.

The issue was fixed by putting a G17 in the positioning of the chamfering toolpath, yet the previous toolpath was in G17, and the active G commands for the chamfering showed in G17. There was no plane rotation or dynamic work offset programmed.

Somehow the machine ignored the G17 from the previous operation, or reset it, yet still showed G17 active.

Has anyone else encountered this? As usual, the machine tool supplier was about as useful as a bowler hat with sleeves...

CNCAppsJames · May 27, 2025, 06:55 PM

Perhaps it may be adjudicated good idea to add a bunch of cancelation codes to the toolchange MACRO as a precaution.

JM2CFWIW

TSmcam · May 27, 2025, 07:06 PM

Quote from: CNCAppsJames on May 27, 2025, 06:55 PMPerhaps it may be adjudicated good idea to add a bunch of cancelation codes to the toolchange MACRO as a precaution.

JM2CFWIW

I agree. Weird nonetheless though. I've never encountered this in all my years of dealing with Fanuc.

The customer noted that if the program was run all the way through, it gouges. If he just restarts at that operation, it cuts fine. All the while, G17 is showing up active.

Truly bizarre.

CNCAppsJames · May 27, 2025, 08:17 PM

What if they run with optional stops? Gouges still?

JParis · May 28, 2025, 02:04 AM

Safety block for every toolpath...

G0 G17 G40 G80 G90

Maybe TS posts can't do that?

gcode · May 28, 2025, 05:42 AM

Quote from: JParis on May 28, 2025, 02:04 AMMaybe TS posts can't do that?

Well, that was rude

Jeff · May 28, 2025, 06:00 AM

On our new Hyundai with the new Fanuc IHMI control I've noticed some strange issues related to the G80 being the culprit, but is fine on our older Fanuc 0-M.
I can't remember what I did to fix it or if this example is the fix it's been so long.
But this is how my post spits out a drill path then a chamfer path, it's just a quick dummy path I whipped up:

Code Select

%
O1234
(XXX)
(MASTERCAM-2025)
G00 G90 G17 G20 G40 G80
G91 G28 Z0.
G28 X0. Y0.
N1
(DRILL--)
(MAXIMUM OPERATION DEPTH = 3.)
(MINIMUM OPERATION DEPTH = -2.)
(T1 - SANDVIK 304SS DE10-15.1-150-M5 2334 - H1 - D1 - DIA .5945")
T1 M06
T2
G00 G90 G54
/M50
S1266 M03
X0. Y0.
G43 H1 Z3.
G94
G98 G81 X0. Y0. Z-2. R.1 F8.48
G80
G49
M09
M05
G91 G28 Z0.
G28 X0. Y0.
M01
N2
(CHAMFER)
(MAXIMUM OPERATION DEPTH = 3.)
(MINIMUM OPERATION DEPTH = -.15)
(T2 - HARVEY 908440-C3 5FL 5/8 CHAMFER MILL - H2 - D2 - DIA .625")
T2 M06
T1
G00 G90 G54
/M08M46
G94
G05.1 Q1 R3
S3056 M03
X.5052 Y1.1919
G43 H2 Z3.
Z.25
G01 Z-.15 F150.
X.4168 Y1.2803 F30.56
G03 X.3284 Y1.3169 I-.0884 J-.0884
G01 X-2.6801
G03 X-2.7685 Y1.2803 I0. J-.125
G01 X-2.8569 Y1.1919
G00 Z3.
G49
M09
G05.1 Q0
M05
G91 G28 Z0.
G28 Y0.
M30
%

TSmcam · May 28, 2025, 12:53 PM

Quote from: CNCAppsJames on May 27, 2025, 08:17 PMWhat if they run with optional stops? Gouges still?

Yes, the optional stop doesn't affect it. Something is "clearing" the plane or affecting it.

TSmcam · May 28, 2025, 12:55 PM

Quote from: JParis on May 28, 2025, 02:04 AMSafety block for every toolpath...

G0 G17 G40 G80 G90

Maybe TS posts can't do that?

LOL, cheap shot

Funny, Mastercam posts dont have that on every toolpath...

TSmcam · May 28, 2025, 12:56 PM

Quote from: gcode on May 28, 2025, 05:42 AMWell, that was rude

I was going to ask how the MT is going, and whats it like having solid models for tools now, but yeah, nah LOL

TSmcam · May 28, 2025, 01:02 PM

Quote from: Jeff on May 28, 2025, 06:00 AMOn our new Hyundai with the new Fanuc IHMI control I've noticed some strange issues related to the G80 being the culprit, but is fine on our older Fanuc 0-M.
I can't remember what I did to fix it or if this example is the fix it's been so long.
But this is how my post spits out a drill path then a chamfer path, it's just a quick dummy path I whipped up:

Code Select Expand
% O1234 (XXX) (MASTERCAM-2025) G00 G90 G17 G20 G40 G80 G91 G28 Z0. G28 X0. Y0. N1 (DRILL--) (MAXIMUM OPERATION DEPTH = 3.) (MINIMUM OPERATION DEPTH = -2.) (T1 - SANDVIK 304SS DE10-15.1-150-M5 2334 - H1 - D1 - DIA .5945") T1 M06 T2 G00 G90 G54 /M50 S1266 M03 X0. Y0. G43 H1 Z3. G94 G98 G81 X0. Y0. Z-2. R.1 F8.48 G80 G49 M09 M05 G91 G28 Z0. G28 X0. Y0. M01 N2 (CHAMFER) (MAXIMUM OPERATION DEPTH = 3.) (MINIMUM OPERATION DEPTH = -.15) (T2 - HARVEY 908440-C3 5FL 5/8 CHAMFER MILL - H2 - D2 - DIA .625") T2 M06 T1 G00 G90 G54 /M08M46 G94 G05.1 Q1 R3 S3056 M03 X.5052 Y1.1919 G43 H2 Z3. Z.25 G01 Z-.15 F150. X.4168 Y1.2803 F30.56 G03 X.3284 Y1.3169 I-.0884 J-.0884 G01 X-2.6801 G03 X-2.7685 Y1.2803 I0. J-.125 G01 X-2.8569 Y1.1919 G00 Z3. G49 M09 G05.1 Q0 M05 G91 G28 Z0. G28 Y0. M30 %

Funnily enough, I suspect it is the G80 too.

They did ask their machine tool dealer, who is some kind of Masterscam dealer. Typical response was "what kind of post is that" or "that code is sh**". Typical MC fangirl response of course

. Seriously though, pretty poor help. They didn't provide any help other than blaming TopSolid, yet this post was proven on an earlier Doosan mill with a very slightly earlier control.

The G17 should be modal, and weirdly the machine displays G17 as active in the problem toolpath. Yet it somehow cancels or changes it. I haven't been able to visit the customer site, but they've found a workaround.

JParis · May 28, 2025, 01:08 PM

Quote from: TSmcam on May 28, 2025, 12:55 PMLOL, cheap shot Funny, Mastercam posts dont have that on every toolpath...

Mine do

But you DO have cookies I have heard lol

TSmcam · May 28, 2025, 01:21 PM

Quote from: JParis on May 28, 2025, 01:08 PMMine do

But you DO have cookies I have heard lol

Yeah, and the cookies taste great.

The standard Mastercam posts dont, and in my years of working with posts a "safety line" code like that was never needed, on any of the machines I have worked with, including the Fanuc 31i. And up until now, non of my TopSolid posts have needed it either.

The machine tool dealers response was expected of course. There are good ones, and substandard ones. This one fits in the substandard basket well

TSmcam · May 28, 2025, 01:52 PM

Quote from: Jeff on May 28, 2025, 06:00 AMOn our new Hyundai with the new Fanuc IHMI control I've noticed some strange issues related to the G80 being the culprit, but is fine on our older Fanuc 0-M.
I can't remember what I did to fix it or if this example is the fix it's been so long.
But this is how my post spits out a drill path then a chamfer path, it's just a quick dummy path I whipped up:

Code Select Expand
% O1234 (XXX) (MASTERCAM-2025) G00 G90 G17 G20 G40 G80 G91 G28 Z0. G28 X0. Y0. N1 (DRILL--) (MAXIMUM OPERATION DEPTH = 3.) (MINIMUM OPERATION DEPTH = -2.) (T1 - SANDVIK 304SS DE10-15.1-150-M5 2334 - H1 - D1 - DIA .5945") T1 M06 T2 G00 G90 G54 /M50 S1266 M03 X0. Y0. G43 H1 Z3. G94 G98 G81 X0. Y0. Z-2. R.1 F8.48 G80 G49 M09 M05 G91 G28 Z0. G28 X0. Y0. M01 N2 (CHAMFER) (MAXIMUM OPERATION DEPTH = 3.) (MINIMUM OPERATION DEPTH = -.15) (T2 - HARVEY 908440-C3 5FL 5/8 CHAMFER MILL - H2 - D2 - DIA .625") T2 M06 T1 G00 G90 G54 /M08M46 G94 G05.1 Q1 R3 S3056 M03 X.5052 Y1.1919 G43 H2 Z3. Z.25 G01 Z-.15 F150. X.4168 Y1.2803 F30.56 G03 X.3284 Y1.3169 I-.0884 J-.0884 G01 X-2.6801 G03 X-2.7685 Y1.2803 I0. J-.125 G01 X-2.8569 Y1.1919 G00 Z3. G49 M09 G05.1 Q0 M05 G91 G28 Z0. G28 Y0. M30 %

Yes, it will be something similar.

We fixed it by adjusting the line similar to yours above to:

G00 G17 G90 G54

Weirdly though, before that line, it showed the G17 active.

CNCAppsJames · May 28, 2025, 04:10 PM

What CNC Series and Edition Software does the machine have?