I cant figure out for Fuison360 to generate the M6 (tool change command)?
Is this your first time using it to machine a part/toolpath?
Is it the non-license version?
Which Masso software version are you running?
Which post processor are you using?
Yes, new to the CNC world. Familiar with CAD and 3 D printing.
It is the licensed version of F360.
Masso and Onefinity post should be on newest version
Can you share the gcode that is being generated?
Be sure that you’re using the masso post processor and not the onefinity.
1 Like
OK, I have not tried the Masso Post yet.
Will do that.
1 Like
Even using the Masso Post I do not get a M6 code:
(1001)
(T1 D=0.25 CR=0. - ZMIN=1.02 - FLAT END MILL)
(T2 D=0.0625 CR=0. - ZMIN=2.02 - FLAT END MILL)
N10 G90 G94 G17
N15 G20
N20 G28 G91 Z0.
N25 G90
(2D POCKET1)
N30 M5
N35 M0
(MANUAL TOOL CHANGE TO T1)
N40 S16000 M3
N45 G17 G90 G94
N50 G54
N55 G0 X1.4702 Y1.5933
…
N4175 G90
(2D POCKET2)
N4180 M5
N4185 M0
(MANUAL TOOL CHANGE TO T2)
N4190 S16000 M3
N4195 G17 G90 G94
N4200 G54
N4205 G0 X8.2584 Y3.5586
Using the Onefinity Post with M6 option checked:
%
(123)
(T1 D=0.25 CR=0 - ZMIN=1.02 - FLAT END MILL)
(T2 D=0.0625 CR=0 - ZMIN=2.02 - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0
(2D POCKET1)
N25 M0
(MANUAL TOOL CHANGE TO T1)
N30 S16000 M3
N35 G17 G90 G94
…
N4165 G53 G0 Z0
(2D POCKET2)
N4170 M0
(MANUAL TOOL CHANGE TO T2)
N4175 S16000 M3
N4180 G17 G90 G94
N4185 G54
It seems the issue is in the tool configuration.
Having 'Manual Tool change" selected seems to suppress the M6 output.
1 Like
Is there any other method than a NC Passthrough to force an M6 tool change before stating the cut (to verify the right tool is installed)?
It looks like you are still using the Onefinity post processor.
Did you try the one from Autodesk - from following the link I provided. I believe @hinro133 above mentioned not using the Onefinity PP as well.
Give that one a try and see if it works.
2 Likes
As noted I tried both post processors
Is it possible for you to share the Fusion file and toolpath you are trying?
I use Fusion - non-licensed - but could try to post a toolpath with one tool to see if I get an M6.
I ran into the same problem with no M6 and realized I was using the buildbot post instead of the MASSO.
It might be a little overwhelming at first glance, but you can open the post (the .cps file), ignore the contents, and search for strings such as masso using “ignore case”. This will allow you to positively identify you have the correct post processor. The MASSO post processor does NOT have an “Output M6” checkbox in the screenshot you showed above.
Once you are sure that the correct one is selected, use it to post process the model to an empty folder to make sure you are not looking at an old output run. Fusion is written using a cross-platform library that is very unintuitive and it is easy to think that you regenerated the file you are viewing when it actually stashed the file somewhere else – and you are still looking at the old file… generating the file to an empty folder and the file being created there as expected makes sure it’s the file you think it is.
To be sure, I always check the modification dates of post processed files to ensure they are sane.
1 Like
Just checking in to see if Tim resolved this issue? I seem to have the same problem.
I downloaded the post processor from Masso, uploaded the .cps in the assets folder in Fusion360 and use it to export the gcode. Also for me, on tool change, it provides an M0 and not a M6.
2D CONTOUR3)
(…)
Y26.35
G3 X358.9 Y26.95 I-0.6 J0.
G1 X358.3
G18 G3 X357.7 Z8.1 I0. K0.6
G0 Z30.
G17
G53 G0 Z0.
(FACE1)
M5
M0
(MANUAL TOOL CHANGE TO T99)
S12000 M3
G17 G90 G94
G54
G0 X393.4 Y7.292
Z30.
G0 Z20.
G1 Z18.6 F300.
G18 G3 X389.8 Z15. I-3.6 K0. F2500.
G1 X388.01
X-18.01
(…)
Just thinking about this, could this be because the machine does not have an ATC (yet)? Hence it uses an M0.
As far as I have understood, machines equipped with an ATC, tool changes might be managed automatically without needing an M0 for a manual pause. Instead, an M6 command would be used to signal an automatic tool change.
The M6 not coming up was fixed by removing manual tool change on the used tools:
Not having the M6 at the beginning of the code, I fixed with editing the post processor (I can share it later)
It seems the issue is in the tool configuration.
Having 'Manual Tool change" selected seems to suppress the M6 output.
1 Like
temp 2.cps (87.9 KB)
Here is the file, use at your own risk.
But basically it inserts an M6 for the first tool used.
If that tool is already loaded the Masso ignores it, otherwise it prompts you for a tool change.
This way you dont have to worry having the right tool loaded when you start the job.
1 Like