[LuthierWizard]

Hey everyone. I'm a guitar builder who took a CNC guitar building course last year. We used Sprutcam 7 for all our CAM needs when I was at the school. I got quite good with the programming but we never went over the postprocessor that much. I now have a Zenbot 48x48 CNC machine with Mach3 as the controller and I have Rhino 5 as the drawing software. I'm just about to drop the money for the CAM software. What I'm a little confused about is Sprutcam's post processor and if I'll have to buy any additional software to get it to work with Mach 3 and the table I have. From what I understand Sprutcam has a built in post processor where as programs like Gibbscam you have to buy additional software to do the post processing. So if I drop $2100 for Sprutcam 8 expert will I be good to go right away to generate G code that will work with my CNC table?

[Bryan Turner]

My version of SprutCAM came with the Tormach post-processor, the Tormach uses Mach 3 as the controller. I assume if you purchase from sprutcamamerica.com, they will give you the Tormach post in the deal.

Alternatively, I'm told Mach works fine with most Fanuc posts, but you should verify before purchase (just ask your salesperson at Sprut).

Most CAM companies will include a post for your machine if you purchase from them, or give you technical assistance in building a post.

--Bryan

[MichaelHenry]

Tormach used to sell two versions of SprutCAM - one that only worked with a Tormach post and another that would work with "all posts". If they still sell both, you probably want the latter. I believe that it (the all-post version) also came with a postprocessor editing utility so that you could modify or create your own posts.

Mike

[mountaindew]

I would check sprutcam website for list of machine post processors that are supported.
a tormach post would not have the right specs..... 48x48

[Bryan Turner]

Mountaindew,

The size of the machine is irrelevant to the post-processor. It's just converting the internal SprutCAM command language into commands that Mach 3 understands - how to perform tool changes, whether to use arcs or straight lines for curves, various restrictions on number of axis moving at one time, spindle, coolant, axis-brake, etc.. Some advanced post processors will give you a warning if the posted code moves outside the machinable area, but really that's the CAM's job and you can set this up in the machine configuration in Sprut. If I recall correctly, mine came configured with 100,000 inches of machinable area!

--Bryan

[mountaindew]

Mountaindew,

The size of the machine is irrelevant to the post-processor. It's just converting the internal SprutCAM command language into commands that Mach 3 understands - how to perform tool changes, whether to use arcs or straight lines for curves, various restrictions on number of axis moving at one time, spindle, coolant, axis-brake, etc.. Some advanced post processors will give you a warning if the posted code moves outside the machinable area, but really that's the CAM's job and you can set this up in the machine configuration in Sprut. If I recall correctly, mine came configured with 100,000 inches of machinable area!

--Bryan

I said a tormach post processor for sprutcam wont make g-code to drive a zenbot 48x48.
And that's incorrect.?
So my 100's of tormach g-code files will run on a zenbot 4848 un altered?
cool.

[Bryan Turner]

Mountaindew,

Just to test it, I ran the same project with Sprut posting to Tormach and to Fanuc, here's the output up to the first few cuts. (I just cut this project using the Tormach post so I know it's working)

TLDR: Basically they're the same code. Tormach post includes line numbers (Nxxx) and posts coordinates into the ten-thousandths, while the Fanuc rounds to the thou. The Fanuc post sets millimeters (G21) instead of inches (G20), which is incorrect so something is not set right in the project or post.

Tormach
-------------------
%
OMY PROJECT NAME

( POSTPROCESSOR: )
( GENERATED BY SprutCAM )
( DATE: 3/19/2014 )
( TIME: 3:30:08 PM )

(Tool) (1) (Diameter)(0.063) (Engraver L0.25, D0.063, A45, dm0, H0.031) (Operation) (Engraving)
(Tool) (1) (Diameter)(0.005) (0.01 End Mill) (Operation) (Pocketing)
(Tool) (3) (Diameter)(0.125) (1/8 End Mill) (Operation) (2D contouring)

N10 G90 G64 G50 G54 G80 G17 G40 G49
N20 G20 (Inch)
(Engraving)
N30
N40 T1 G43 H1 M6
(Engraver L0.25, D0.063, A45, dm0, H0.031)
N50 S10000 M3 M8
N60 G0 G94 X0.8092 Y-0.3716 Z0.1 A0.
N70 Z0.0087
N80 G1 Z-0.0063 F4
N90 X0.809 Y-0.3711 Z-0.0063 F80
N100 X0.8047 Y-0.3567 Z-0.0049
N110 X0.8045 Y-0.3563
N120 X0.8044 Y-0.3559 Z-0.0049
-------------------------------

Fanuc
--------------------------------
%
<MY_PROJECT_NAME>

( GENERATED BY SprutCAM )
( DATE: 3/19/2014 )
( TIME: 4:31:36 PM )

( TOOLS LIST )
( T1 ENGRAVER D0.063 )
( T1 CYLINDRICAL_MILL D0.005 )
( T3 CYLINDRICAL_MILL D0.125 )

G90 G00 G21 G40 G49 G69 G80 G17

( ENGRAVING )
G53Z0.
G53X0.Y0.
T1M6 (ENGRAVER L0.25, D0.063, A45, DM0, H0.031)
G54
G17
S10000M3
G00G43H3X0.809Y-0.372Z0.1A0.
Z0.009
M8
G01G94Z-0.006F4
F80
X0.805Y-0.357Z-0.005
Y-0.356
Y-0.355
Y-0.354
X0.804Y-0.348Z-0.006
Y-0.347
Y-0.347
X0.805Y-0.346Z-0.005
Y-0.346
----------------------------------

Here's a g-code reference to follow along (LinuxCNC "G-Code" Quick Reference).

Stripping comments, line numbers, and coordinates, the commands between start and cutting metal are (this is NOT valid g-code anymore!).

Tormach:
G90 G64 G50 G54 G80 G17 G40 G49 G20 T1 G43 M6 S10000 M3 M8 G0 G94 F4 F80

Fanuc:
G90 G00 G21 G40 G49 G69 G80 G17 G53 T1 M6 G54 G17 S10000 M3 G00 G43 M8 G01 G94 F4 G1 F80

Sorting the codes lexicographically, we can more easily see the differences:

Tormach:
F4 F80 G0 G1 G17 G20 G40 G43 G49 G50 G54 G64 G80 G90 G94 M3 M6 M8 S10000 T1

Fanuc:
F4 F80 G00 G01 G17 G21 G40 G43 G49 G53 G54 G69 G80 G90 G94 M3 M6 M8 S10000 T1

Differences:
G0 is the same as G00
G1 is the same as G01
G20 = set units to inch
G21 = set units to mm
G50 = reset scale factors to 1.0
G53 = set coordinate system to machine coordinates
G64 = "best speed path" or "constant velocity mode"
G69 = cancel coordinate rotation

So basically, they're the same.. slightly different order for setting up the machine, and each does a bit of cleanup that the other does not (clear scale factors, undo coordinate rotation, etc).

Finally, I ran the Tormach post on a simple geometry of a 20" circle (way out of the Tormach limits) with a profile cut all the way around and it posted fine, so the post doesn't care about the machine limits (Sprut complained, as expected).

Hope that helps!
--Bryan

[mountaindew]

Hey Brian thanks for detailed explanation.
After thinking about that all day yesterday, I kind of figured out g-code is very generic and would run ok for the most part.
If g-code was set for cutting cabinet door panels and run on my machine it would just take off and hit limits.
Learning more every day
Thanks again for info!