Exporting Tool Settings

[angusstevenson123]

Hello,

Can anyone help with the problem of exporting tool settings?

Specifically, I do up a design with unique tool settings (eg, 5mm bit, target depth 10mm etc) on my own computer - but when I email the G-Code to my manufacturer - he has to sift through my files and manually re-enter all the tool settings.

Can the tool settings (diameter, target depth etc) be exported to save this re-work by the manufacturer?

Any help or guidance much appreciated.

Thankyou - Angus.

[lloydsp]

Angus,
A simple way to do that would be to prepare a post-build processor or just a simple shell script that will parse out the tool settings from a g-code file, and write only those lines to a new file.

I think it would be preferable to do it with the post-build process, since that way, every time you generate g-code, you'd also update the tool settings file.

LLoyd

[Jeff_Birt]

When I set up a job I have a print out of and engineering drawing in front of me that I write down each tool used and its maximum DOC. In the MOP name I record the tool used, for example a MOP name might be" Center Pocket, 0.125EM, 0.25DOC". Then when I go to the machine I know what tools I need to use. Since your working with an outside manufacturer it seems the best way to go would be to assign a dedicated tool number to each tool used, so your MOP name would be "Center Pocket Tool 5". Then your tool number in the MOP would be Tool 5. You would just need to provide a table of these standard tools to the manufacturer.

In the Mach3-CutViewer post it puts a list of the tool numbers/diameters used in the top of the GCode file so it is easy to see by looking at the file what is used.

Your manufacturer may already have a set of tooling they keep installed by default on their machines. If you find out what this is you may be able to set up your GCode to use their default tooling and save them time and you money.

[pixelmaker]

If you give out the G-code from cambam and use one of the delivered post processors you get a list of the used tools in the header of the nc file, e.g.:
( T3 : 3.0 )
( T8 : 4.0 )
This shows the tool number and the diameter.
The manufacturer has not to know the target depth and any other values for the tool.
other values ​​are dependent on the machine and the material and not have to interest the manufacturer.
He has to tell you with which values he can work.

ralf

[Jeff_Birt]

The manufacturer has not to know the target depth and any other values for the tool.

ralf

They sure do need to know the target depth! There is a big difference in tool selection, i.e. a stub mill may be used and provide faster cutting and better finish when its DOC if sufficient. But then you may need a deep reach tool in other cases. The maximum DOC is a vital piece of information.

[pixelmaker]

The maximum DOC is a vital piece of information.

I'm in your opinion. But this is a information that the manufacturer has to give to the CAM worker. I can´t make a cam file with my values and the manufacturer don´t have the tools or can´t work with my speeds.

All values from the tool library you can give out in to the tooltable. Each item in the list is formatted using the Tool Table Item definition in the post processor.
I think there is no macro for the flute length value. But you can use the Comment line to write every information you want in the tool table with the macro $tool.comment .

ralf

[Garyhlucas]

Ralf,
Yep I used to program for three machines.  When I got a job my first stop was to talk over the desired process with the machinist running the machine.  Second stop was the toolroom to see if we actually had the tools he'd like to use, then another stop back with the machinist to get the okay to use what we've got or order more tools.  Then I'd write the program which was easy once I knew all that other stuff.

[angusstevenson123]

Thanks for everyone's input above - I am quite a novice with CAMBAM and manipulating G-Code and post processors but I have here a possible solution - very labor intensive - but it works for me.

[pixelmaker]

hello angusstevenson123,

nice pdf but wrong name. It should be "Export G-Code" or "Output G-Code".
The G-code you produce is a machining language and has nothing to do with the Cam Styles. The G-Code feeds the controller software.
The Cam Styles are a library of machining datas in CamBam.
After your point 7 in the pdf (manually enter data as follows) you right click on this mop and "Copy".
Then you open your Cam Style Library, make a new Cam Style and "Paste Format".
The values from your mop now stored in the Cam Style, rename it "PERSPEX_NAMPLATES". Next time you want to cut Perspex Nameplates you simply create a new mop, choose the Cam Style and all cutting datas are there.

If you want to use the Cam Styles at a other PC you copy the folder "Styles" from the system folder to the same place of the other PC.

ralf

[lloydsp]

In the case of wanting to export the tool definitions to an external file, here are some hints:

The modifications below are more easily done by using a text editor to edit the post-processor file, than to use the built-in editor in CB.


The first thing you need to do is modify your post-processor to output the tool-specific information in a comment before each MOp, thus:
------------------------
  <ToolTableItem>{$comment} T{$tool.index} DIA {$tool.diameter} {$endcomment}</ToolTableItem>
  <ToolChange>
{$comment} TOOL/MILL, T={$tool.index},DIA={$tool.diameter},LEN={$tool.length},PROF={$tool.profile} {$endcomment}
M5  ; spindle off
M25
G28 ; Go To Machine Return Position
{$comment}{$part.name} -- {$mop.name}{$endcomment}
{$comment} T{$tool.index} {$tool.diameter} {$tool.profile} {$endcomment}
T{$tool.index} M6
G43 H{$tool.index}
</ToolChange>
  <MOP>
{$toolchange}
...
----------------------------------------------------


It will result in this sort of output in the g-code (snippet):
------------------------------------------
%
O1
: CONSOLE LAYOUT3
:
: CAMBAM
: CONSOLE LAYOUT3 10/4/2014 9:09:10 AM
: T1 DIA 0.005
: T2 DIA 0.125
: CUTVIEWER
: FROM/0,0,5
: STOCK/BLOCK,,,,,,
G20
G0 G17 G40 G80 G90
: TOOL/MILL, T=1,DIA=0.005,LEN=2.5,PROF=VCUTTER
M5  ; SPINDLE OFF
M25
G28 ; GO TO MACHINE RETURN POSITION
:LABELS -- ENGRAVE1
: T1 0.005 VCUTTER
T1 M6
G43 H1
:LABELS -- ENGRAVE1
G0X-0.7134Y1.4467
S3000 M3
G4 P6
...
---------------


Then you can invoke an external script or program of your choice to parse the g-code by modifying the post (at the very bottom) thus:

  <PostBuildCommand>myscript_or_program_that_uses command-tail_arguments</PostBuildCommand>
  <PostBuildCommandArgs>{$cbfile.name}.nc</PostBuildCommandArgs>
  <SuppressParserErrors>true</SuppressParserErrors>
</PostProcessor>

That's the way I do it.
LLoyd