Fagor 8055 Mill Sample Code and Helical Interpolation

[sailcam]

Can someone please help me with some sample code for a Fagor 8055 Mill controller, so I can edit a post processor.

I need the sample code to include:
1) Prepatory codes and formats
2) helical motion code as it fails on the helical ramping code (spiral ramp entry to a cutter path)below with an error something like "incorrect code"
G03X-20.928Y36.248Z83.273I4.256J2.109

I assume this controller can do helical ramping

I have had it running with basic X Y Z linear commands

am I missing a prepatory code for cutter tip output or a G40 offset cancel or something???

below is a sample of the start of the CAM generated code I'm trying to get to run (n.b. cutter tip output, not C/L):

%
G21
G17G90
F5000
( Waterline Toolpath 1 [16x3, 0.3] )
( Waterline Toolpath )
( Cutter: 16.000x3.000 )
( Note: Cutter tip output )
G01Z91.000
G01X-28.292Y39.732
T1M06
G00G43Z91.000D1
G00X-28.292Y39.732
S7500M03
M07
G01Z86.612
F1500
X-28.275Y39.697Z86.215
X-28.223Y39.592Z85.835
X-28.138Y39.421Z85.485
X-28.024Y39.192Z85.180
X-27.886Y38.913Z84.932
X-27.729Y38.595Z84.750
X-27.558Y38.252Z84.642
G03X-20.928Y36.248Z83.273I4.256J2.109
G03X-19.189Y42.736Z81.958I-2.375J4.114
G03X-25.678Y44.475Z80.642I-4.114J-2.375
G01X-26.157Y44.198
X-26.694Y43.892
G02X-28.082Y43.356I-2.474J4.345
G01X-28.594Y43.242
F5000
Z91.000
M09
M05
M02
%

Thanks in advance for any assistance is much appreciated by myself and customer!

[cut more]

Sailcam,
I run a Fagor 8050 on a Motionmaster Router. I have not tried Helical Ramping but I do use Tool length Comp.
(n.b. cutter tip output, not C/L): Not sure what you mean by n.b. cutter tip output?
What is this machine z91! F5000! Scary.

Try these changes,
T1 D1
M06
G43 D1
Sample of what I use.
M5
T03 D3; T-Spoke cutter Z-25.7937at tabletop
M6
M51
S12000
M3
G55;my work offset
G43 D3
X5.5 Y58. Z17.5
G01 Z14.4273F50
X57.5 Y6.F30
G00 Z17.5
Y58.
G01 Z14.4273F50
X5.5 Y6.F30
G00 Z17.5 M5
G44 Z0

I do know my control will read up to 30 lines ahead so your error is not neccessarily on the line it stops at.
What software are you using to post with? I use bobcad and it has a decent post.

[sailcam]

Firstly, thanks for the reply Cut More!

>(n.b. cutter tip output, not C/L): Not sure what you mean by n.b. cutter tip >output?

The Software that generated the code is High Speed Machining based, so rather than use the CNC's offset (which doesn't calculate the tip rad. on a hognose or ballnose cutter), the software calculates the tools position relative to where the tool tip touches (tangentially) the finished surface of the part.

>What is this machine z91! F5000! Scary.
That's the rapid to the safe height above the part, usually it's F10000 (but remember where mm's down under!)

>Try these changes,
>T1 D1

Maybe I need to leave the D1 out so there's no controller based rad compensation, or use a G40 (Compensation Cancel) between here and the G43 height offset.

>M06
>G43 D1
>Sample of what I use.
>M5
>T03 D3; T-Spoke cutter Z-25.7937at tabletop
>M6
>M51
>S12000
>M3
>G55;my work offset
>G43 D3
>X5.5 Y58. Z17.5
>G01 Z14.4273F50
>X57.5 Y6.F30
>G00 Z17.5
>Y58.
>G01 Z14.4273F50
>X5.5 Y6.F30
>G00 Z17.5 M5
>G44 Z0

>I do know my control will read up to 30 lines ahead so your error is not neccessarily on the line it stops at.
The controller looks ahead also, but still shows the error to be on the line of code that is incompatible i.e.- the first helical interpolation move:

G03 X-20.928 Y36.248 Z83.273 I4.256 J2.109

Maybe, it prefers G3 to G03, but I'd be surprised if it can't read either format.

Still would like to hear from anyone who uses Helical Interpolating High Speed Machining based code on this controller.

Thanks!

[cut more]

Sailcam,
>Maybe I need to leave the D1 out so there's no controller based rad compensation, or use a G40 (Compensation Cancel) between here and the G43 height
G44 is the tool length cancel, Tool rad. Comp.(G41, or G42) will only be active if called even when the D# is in the program.You can tell if any comps are active by looking at the controller lower left where all active codes are displayed.
Are you using G21 as programming in mm.?
My Fagor manual for the 8055M tells me that is the code for Definition of an upper work zone limit and G71 is Programming in mm. G70 is programming in inches.
The control will read eitheer G03 or G3 I use G3 because it saves 1 little bit of memory and I need all I can get.
Hope I am helping.