Tilted 4th Axis Tormach

[Anonymous]

I am quite new to CAM and of course, started out with a tilted 4th axis part! I have some horizontal 4th axis operations (rotary table on right side of the machine in line with X) that make nice looking tool paths that also post-process w/o issue. I am still setting up my Tormach 1100M so I don't know yet how it will run...

I have been going in circles with the tilted 4th axis. I need it tilted to get a small tool in between the teeth. I can get good looking tool paths (also look good when simulating) with the Multi-Axis Flow operation, but it won't post-process. See pictures below:

ISO ViewFront View

It gives the following error when I post-process:

Information: Configuration: Tormach PathPilot
Information: Vendor: Tormach
Information: Posting intermediate data to 'C:\Temp\PostProc\1001.nc'
Information: Total number of warnings: 3
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Thursday, May 23, 2019 11:10:38 AM
Warning: function getProgramNameAsInt does not always return a value
Warning: function getProgramNameAsInt does not always return a value
Warning: function getProgramNameAsString does not always return a value
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.3.0 45221
Configuration path: C:\Temp\PostProc\tormach.cps
Include paths: C:\Temp\PostProc
Configuration modification date: Monday, May 20, 2019 9:50:08 PM
Output path: C:\Temp\PostProc\1001.nc
Checksum of intermediate NC data: bb0820b50cae0715a4acda487fdc9fb6
Checksum of configuration: fb5d9ddfe1ea92e237772e2f17a41e84
Vendor url: http://www.tormach.com
Legal: Copyright (C) 2012-2018 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.5790
...

###############################################################################
Error: Error: Direction is not supported for machine configuration.
Error at line: 1

Stack dump:
("Direction is not supported for machine configuration.")@:0
onOpen()@C:\Temp\PostProc\tormach.cps:242
Failed while processing onOpen().
###############################################################################

Error: Failed to invoke 'onOpen' in the post configuration.
Error: Failed to invoke function 'onOpen'.
Error: Failed to execute configuration.
Stop time: Thursday, May 23, 2019 11:10:38 AM
Post processing failed.

I tried the 4-axis limit option through "4-axis Limit" beta mode option and it doesn't work for this one. It does work for some of my horizontal 4th axis operations.

I feel like it has something to do with the setup WCS and/or tool orientation, but I don't fully understand the implications of both of those. For the horizontal 4th axis operations that worked, I put the setup WCS in same direction as the machine's axes and put the tool orientation with the Z axis lined up with the rotary table axis.

When I do that with the tilted axis setup, the tool is at a weird angle and it doesn't post process. The tilted axis is a different cut: the horizontal axis tool path wraps around the whole part, the titled 4th axis op only does a pocket.

After writing all this up, I realized I have one good tooth space tool path. I might try post-processing that and go through the Gcode and add a repeat loop that would retract the tool, rotate the A axis and repeat the tool path. Or worst-case is I could rotate the part through Path Pilot and re-run the same program 14 times. Obviously, I would much rather fusion would take care of all this and I wouldn't have to manually code or rotate the A axis 🙂

Please explain things to me like I have no idea what I am doing since that wouldn't be too far off from reality. All help is greatly appreciated!

Cheers,

Brett

Windows 10, Suface Pro i7, 8Gb Ram

Tormach 1100M, 6" Tilting Rotary Table

[daniel_lyall]

Can you post this model, To do this Go to File -> Export and save as a .F3D Archive File and attach it to your next post, if you can not post the file you can PM it to me or say in your next post you can not post the file.

It looks like it may be spitting out a 5 axis toolpath 

[Anonymous]

I didn't have an option to create an F3D file under export. I changed the .F3Z file to .ZIP and pulled out three .F3D files, see attached.

Thanks!

Brett

[daniel_lyall]

What size tool are you going to use?

Can you do a save as on this model, name it something else break link of the inserted components then post that file so I can see what you have done with the toolpaths.

[Anonymous]

I am using a 1/16 ball nose tool. Please see attached F3D file that has the broken links.

I don't have the circular pattern in this file. There are 14 teeth, so the pattern is just revolved around the circular base 14 times, which is what I am hoping I can get Fusion 360 to do for me 🙂

Cheers,

Brett

[daniel_lyall · Accepted solution]

Have the WCS in the setup set like what is in the toolpath and untick the tool orientation and model in the toolpath.

What it was doing was going from the orientation in the setup (a C axis Move)to the tool orientation in the toolpath, if the first toolpath is going to be the same orientation as the setup's you do not need set the orientation in toolpath you only set if it is going to be different.

you won't be able to pattern the toolpath in the same orientation as the model it will be a 5 axis move.

[Anonymous]

Thank you, that helps clarify what the WCS setup and toolpath orientation do. Some of this CAM stuff is starting to make sense 🙂

Can I use the Gcode from the one tool path and add a loop like this:

#1=360 / 14

#2 = 0

N100

[GCode generated by Fusion to cut one tooth space here]

#2 = #1 + #2

G0 A#2 (Rotate A axis 1/14 turn... This would have one extra turn at the end, but would be worth it)

IF [#2 < 359] GOTO 100

Rest of Gcode for other features here...

Of course, I need to make sure it has a retract before each 1/14 turn.

Thanks,

Brett

[daniel_lyall · Accepted solution]

When it comes to macros and subs with Linux I would not have a clue, run it through a Gcode simulator like ncviewer https://ncviewer.com/ 

If it looks good chuck it on the machine and sees If it looks ok in the viewer(whatever it is called) to do a dry run to make sure it will be ok.

Just running your G code through ncviwer and looking at it on the machine just to see if it looks ok 9 times out of 10 when you think something looks wrong it will be.

[Anonymous]

Thank you for all your help Daniel! I didn't know about the ncviewer site, I will definitely run it through there, view it on Path Pilot and cut one part made out of air before cutting my first part.

Cheers,

Brett