Tool sequence not correct

[MikeUSNRet]

Ok experts. need some problem solving help with this one.

I saved a gcode that uses 3 tools for the carve and have then numbered as #301, #303, and #201 in that order.

I looked at the .gcode with notepad ++ and see this:

Line 1 T301
Line 50028 M6 T303
Line 484591 M6 T201

Those 3 lines are as they should be. Great right? Not so fast.

I load the file into Carbide Motion (Build 513) and it shows this:

Tools Used #303 #201
First Tool #303

So what about tool #301 which should be up first as per Line 1 of the code?

this is a 3D cut that was modeled in Aspire (10.5) and I DO have a bit setter on my Shapeoko 3 XXL. I suppose I can save 1 gcode per tool, but until just recently, have not had to. (note: my first 3d carve since 10.5 upgrade). Does my Line 1 of the gcode also have to have an M6 called out in it? If so, I can easily edit the post processor for this to be there.

Mike

[MikeUSNRet]

Update:

Solved my issue. ended up modifying the Header of the Post Processor to read "M6 T[T]" instead of just "T [T]" Apparently Carbide Motion cannot read just for a T command and will only recognize the line if it has an M6 as part of it.

[kstrauss]

I don't know the specifics of the Carbide Motion gcode interpreter but the LinuxCNC manual is pretty clear:

Tx - prepare to change to tool x.

The tool is not changed until an M6 is programmed (see Section M6). The T word may appear on the same line as the M6 or on a previous line. It is OK if T words appear on two or more lines with no tool change. Only the the most recent T word will take effect at the next tool change.

Note the highlighted section. The tool is only changed when the M6 command is processed.

[TReischl]

Yup, it is kind of a thing about understanding how g code works.

A "T" word does not cause a tool change to occur, just tells the controller what tool to change to.

The M6 is the actual command to execute a tool change and the control has stored in a register which tool to get.

[Diy_CreatorRH]

Mike , what post processor did you use for your XXL
The on from GitHub?
https://github.com/neilferreri/V-Carve-PPs

I’m Using an XXL And ASPIRE also
Till now I’ve just be load individually
And reversing before I start the job
I’d like to start using the tool changer. And not have to refer o especially when tiling

[Uncle Bob]

Be sure the software you use for machine control accepts automatic tool change and that you have it set for ATC. Check your post processor as well.

I love my ATC.

Bob

[SaltydogWoodworks]

hey Bob,
hoping you could help me out. i've emailed tech support and it would appear as though many people are having the same issue as me..
My router uses centroid acorn and i'm using vectric for tooling. whenever i attempt to save a tool path file using differing cutters, vectric is giving me an error? i've tried using different post extensions, and each time it errors out?
Any help would be appreciated.
Thanks!
Mark

[Adrian]

whenever i attempt to save a tool path file using differing cutters, vectric is giving me an error?

Is the "error" saying that your tools have the same tool number? When saving multiple tools to the same file the tool number must be different for each tool otherwise the machine will have no idea that you want to change tools.

It would really help if you would say what the error actually is. This is the 2nd thread you've raised this issue on and neither time have you stated the error text which makes it hard to offer the exact solution to the problem.