Mill/Turn Post for Fanuc 21i on a CTX410

[mjoconr]

Hi All

So with help from @xander.luciano I was able to draw and CAM out a part which has center drilled holes around the the spun axis.

My problem now is that the generic lathe POST for the fanuc give a single line error of '!Error: Failed to post data. See log for details.' I have not been able to find a log and am a little lost as to the steps I need to take to get the POST to under stand the issue.

The online docs form Autodesk indicate a location for the logs on my mac but there not at this location. With out the logs I can do anything to take this process forward.

I need to adjust the output of the post to give me X and Z axis with a C for the chuck.

A M14 turns on control of the C axis for the chuck

M103 and M104 set the direction of the driven tool (CW, CCW)

I'm sure there is more but at this stage I have no idea.

[xander.luciano]

Hey!

I'm not a mac user so I can't tell you where on mac it might be. Though some google suggesting to open terminal and type: open $TMPDIR

On windows, the CAM logs will be saved to: %localappdata%\Temp\Fusion360CAM\

Thought, the log file show be popping up when you post you operations. Do you have this box checked?

But, in case you can't find the log file, and the NC editor isn't popping up even with that checked, here's what your log file would say (should say):

Information: Configuration: Generic FANUC Turning
Information: Vendor: Fanuc
Information: Posting intermediate data to 'X:\Xander\Desktop\NC Exports\12.nc'
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Thursday, November 3, 2016 5:19:37 AM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41239
Vendor url: http://www.fanuc.com
Legal: Copyright (C) 2012-2016 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2528
...
Error: Milling toolpath is not supported by the post configuration.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke 'onOpen' in the post configuration.
Error: 
Error: Failed to execute configuration.
Stop time: Thursday, November 3, 2016 5:19:37 AM
Post processing failed.

Error: Milling toolpath is not supported by the post configuration

Which is expected as none of our default posts are setup for mill turns. We're gunna need to get you a custom post processor. 

Here's a basic visual of what needs to be done (i.e. how your WCS needs to be, and what the post needs to do):





Anyways, I'm working on a longer post, as well as trying my hand at the post processor for this, but just wanted to acknowledge your post!

Best,

Xander Luciano

[mjoconr]

Hi Xander

I found this PDF in the all the documents I was given which describes the use of the C Axis (The file name was not descriptive). Start from page 93 for details.

Mike

[mjoconr]

Hi @xander.luciano

I looks like that document I attached is as close to 100% wrong as I can find.

I wrote program use the examples and they just fail.

Its looking like the following works I wrote the code for the part you helped with.

M19 (lock spindle at set deg)

M14 (enable C axis)

M15 (disable C axis)

M103 (CW live tool)

M104 (CCW live tool)

M105 (stop live too)

G28 C0 (C to zero deg)

(OD RADIAL DRILL 8 HOLES AT 45DEG)
M1
N410 G55 M8
T1111
M5
M14
M19
G28 C0
N440 G0 X28.5 Z5.
N445 G0 Z-11
N450 G97 S5000 G95 M104
G1 X17.2 F.1
G0 X28.5
C45
G1 X17.2 F.1
G0 X28.5
C90
G1 X17.2 F.1
G0 X28.5
C135
G1 X17.2 F.1
G0 X28.5
C180
G1 X17.2 F.1
G0 X28.5
C225
G1 X17.2 F.1
G0 X28.5
C270
G1 X17.2 F.1
G0 X28.5
C315
G1 X17.2 F.1
G0 X28.5
G0 Z5.
M15
M105