What's new
What's new

Fadal Stops Mid-program

steelrides

Plastic
Joined
Oct 6, 2021
I'm having trouble figuring out why my Fadal is stopping mid-program. I'm running a single-form helical thread-mill operation, which I haven't done before, but it shouldn't be much different than a helical ramp into a pocket. Is there a g-code/m-code that is causing it to jump out of the program? I am running DNC through a Calmotion USB adapter, but that's been fine to date. "sum" doesn't show any new errors.

Details: 1995 Fadal 4020HT 88HS Format2, 94.1 firmware
CAM: HSMWorks in Solidworks with the standard Fadal Post

The last line shown on the screen is N230 and then it goes to Enter Next Command leaving the spindle and coolant running. It does this repeatably. Is N230 the last line read or the next line to perform?

Ideas?

Code:
O8004
(T8  D=0.3125 CR=0. TAPER=118DEG - ZMIN=0.33 - CENTER DRILL)
(T17  D=0.3125 CR=0. TAPER=118DEG - ZMIN=-0.1726 - DRILL)
(T18  D=0.3 CR=0. - ZMIN=-0.12 - FORM MILL)
N10 G90 G94 G17
N15 G20
N20 G28 G91 Z0.
N25 G90

(SPOT DRILL)
N30 T8 M6
N35 S800 M3
N40 G4 P225
N45 M8
N50 G0 E18 X1.5 Y-1.25
N55 G43 Z0.98 H8
N60 Z0.58
N65 G98 G81 X1.5 Y-1.25 Z0.33 R0+0.58 F13.12
N70 X0.75
N75 G80
N80 Z0.98
N85 M5
N90 G28 G91 Z0.
N95 G90

(TAP DRILL)
N100 M9
N105 M1
N110 T17 M6
N115 S3670 M3
N120 M8
N125 G0 E18 X1.5 Y-1.25
N130 G43 Z0.98 H17
N135 Z0.58
N140 G98 G83 X1.5 Y-1.25 Z-0.1726 R0+0.58 Q0.25 F29.
N145 X0.75
N150 G80
N155 Z0.98
N160 M5
N165 G28 G91 Z0.
N170 G90

(THREAD1)
N175 M9
N180 M1
N185 T18 M6
(ALUMINUM THREAD MILLING)
N190 S10000 M3
N195 M8
N200 G0 E18 X0.75 Y-1.25
N205 G43 Z0.98 H18
N210 Z-0.04
N215 G1 Z-0.12 F5.
N220 G41 D18 X0.7175 Y-1.43
N225 G3 X0.8975 Y-1.25 J0.18
[B]N230 X0.6025 Z-0.0888 I-0.1475 F13.7[/B]
N235 X0.8975 Z-0.0575 I0.1475
N240 X0.6025 Z-0.0262 I-0.1475
N245 X0.8975 Z0.005 I0.1475
N250 X0.6025 Z0.0363 I-0.1475
N255 X0.8975 Z0.0675 I0.1475

For example, here's the code for a helical ramp on a finishing perimeter with all the same codes called out, so I'm not sure what's causing the problem.

Code:
(FINISH PERIMETER)
N2130 M9
N2135 M1
N2140 T4 M6
(ALUMINUM FINISHING ON F4020)
N2145 S10000 M3
N2150 M8
N2155 G0 E17 X0.6207 Y0.1298
N2160 G43 Z1.0906 H4
N2165 Z0.6969
N2170 G1 Z0.5787 F20.
N2175 Z0.1431
N2180 G19 G2 Y0.1048 Z0.1181 J-0.025 F37.
N2185 G17
N2190 G1 G41 D4 X0.4832 Y0.0798
N2195 G3 X0.6457 Y-0.0827 I0.1625
N2200 G1 X6.3543
N2205 G2 X6.748 Y-0.4764 J-0.3937
 

Cole2534

Diamond
Joined
Sep 10, 2010
Location
Oklahoma City, OK
Mine gets goofy like that on small arcs, perhaps the tool radius is too close to the arc radius? (.15 and .1475, respectively)

In the back of mind I think there's a command you can hit to add some dialog to the error, but I wouldn't swear to it.
 

in2glamisgirl

Aluminum
Joined
Jun 20, 2006
Location
Hawthorne, CA USA
The program usually does not stop on the problem line due to the look ahead buffer.
I would try without cutter comp as a first step in the trouble shooting process.
 

JonFinn

Aluminum
Joined
Apr 25, 2013
Location
CA, USA
Your second example program does not have any helical moves. There is a G2 while in the G19 plane and a G3 while in the G17 plane, but there are no three axis interpolations.
 

steelrides

Plastic
Joined
Oct 6, 2021
Mine gets goofy like that on small arcs, perhaps the tool radius is too close to the arc radius? (.15 and .1475, respectively)

In the back of mind I think there's a command you can hit to add some dialog to the error, but I wouldn't swear to it.

I removed the cutter comp for troubleshooting, but it was reducing the stepover distance that fixed it. Tool radius was too close and it didn't have the room. Thanks for all the good ideas!
 

Omega

Aluminum
Joined
Nov 3, 2014
Mine gets goofy like that on small arcs, perhaps the tool radius is too close to the arc radius? (.15 and .1475, respectively)

In the back of mind I think there's a command you can hit to add some dialog to the error, but I wouldn't swear to it.

At "Enter next command"...type SUM (enter)...the control will run through the program and check for errors, If it finds any they will list out on the screen
 

Kevinstj

Cast Iron
Joined
Feb 17, 2011
Location
USA
I had a problem with my machine quitting during the DNC Calmotion. I switched from DNC to DNCX and have had no problems since.
 








 
Top