Tool Change

So you are doing a manual tool change, right?
and you have read the SketchUcam help on toolchange? it is linked from the 'New i 1.4' section on the front page of the help.

If you controller understands a 'T1 M6' type of toolchange command, then you can use the first 4 edit boxes to set the parameters for that
OR
you use the next 2 edit boxes to set up a macro file and tool offset.

'tool offset' means that you need to know the difference in length between the first tool and all other tools.
OR between a 'standard tool' and all other tools. The standard tool can be a spacer that you use between the spindle and the work to set Z-zero. Then all tools have an offset relative to that length.

You need to write yourself some G-code that matches your machine and the offset system you want to use.
This code needs to:

• turn the spindle off
• position the spindle somewhere for the tool change
• wait while you change the tool
• set the tool length offset, or probe for the offset, or ????

This might look like this

M05 ; turn spindle off
G49 ; cancel tool length offsets
G53 X200 Y0 Z100 ; go somewhere in machine co-ordinates where tool change can be done
M0 ; wait till resume, NEVER USE a timed delay!
G43.1 Z21.3 ; the 21.3 is the tool length offset for this tool, as compared to your standard tool
G0 Z0 ; this may be needed to make sure the tool offset it in effect.​

In the SketchUcam tool parameters when you specify 'use a tool file' it expects a file like the above code, but with
G43.1 Z%s
instead of an offset number.
The tool length offset you insert in the Tool Offset box will be inserted instead of the '%s'.

In use, each G-code file for each tool will be generated separately, and then joined using the joiner tool.
(Gplot will not like the G43.1 line and will not display the code, the basic cut code is going to be fine, but you must test your tool change code very carefully.)

oh! just spotted a problem in the help example, the G38.1 should be the G43.1 as above. G38.1 is a probe cycle which you can only use if you controller supports it (in the case of GRBL, it does, but the GUI software has to support it as well)

'standard tool' is usually your longest tool so that all other tools are shorter and thus a negative offset. This provides some safety against crashing in that if you enter the wrong offset, the tool is likely to be too short to hit anything before you figure it out and hit Estop.
You must set Z-zero using the standard tool

I have been googling and there is, so far, no good example of using tool changes other than with Mach3 and LinuxCNC.

 

AFAIK You can only do this if you keep your G-code files per tool separate, ie, do not join them and in fact do not use a tool change macro at all.
The reason for this is that when the controller is in 'M0' pause mode you cannot jog and set zero.
Thus you have to set up the tool, then run the Gcode for that tool.

However, do google the MAch3 manual tool change macro facility.

Even better, install a tool height sensor (-:

 

No. The code wont work with Control. You'll need to create separate files for each tool change. Run the first file, change tools, probe Z only, then run the next file. Rinse and repeat.

 

Rather use one of the compatible CAMs: docs:software:overview [OpenBuilds Documentation]

 

Then refer to the others, like Fusion 360 - for which our Post also creates seperate tool files for you: docs:software:fusion360 [OpenBuilds Documentation] or Vectric (which has a tickbox for seperate toolfiles in the Toolpath window): docs:software:vectric [OpenBuilds Documentation]

See docs:software:overview [OpenBuilds Documentation]

 

Basic entry level CAM software is included yes, but nothing beats the power of a real CAM - its a worthy upgrade - when you want to start doing advanced work requiring toolchanges etc. Then its time to use an advanced CAM as well. We provide posts and support for those too

 

Yes, you forgot to set a Coordinate system under WCS in the SETUP > Post Process tab How to define Work Coordinate Systems in Fusion 360 Manufacture | Fusion 360 | Autodesk Knowledge Network
Set it to 0 (first work coordinate system) if you are unsure: 0 = G54, 1 = G55, 2 = G56, 3 = G57 etc - you can layer jobs across multiple coordinate systems (advanced use case, typical for jigging setups)

 

Ahh sorry, yes, correct

 

When you set it to 1, right click on 1 and click "set as default". Then all new setups will automatically put 1 in there for you.

 

Did you home your machine first? The first move relies on a homed machine. If so, then perhaps you dont have enough clearance for the first move. The first move need 10mm between your stock and your Z limit switch. If you dont have that much clearance, you can try changing your Z start and end position in the post processor properties dialog box to -5.

 

There are multiple coordinate systems
G53 = Machine Coordinates = set by homing
G54-G59.1 = Work Coordinates = set by probing and zeroing

Fusion uses both Machine and Work coordinates

G53 G0 Z-10 (or Z-0.3937 in inch) means: RAISE Z up to "10mm below the Z homing switch" - as it moves in the G53 coordinate system

Forgetting to home means moving to "10mm below the switch" looks like a random move, and may even plunge down causing an accident - as G53 (Machine Coordinates) was not established. ALWAYS HOME before setting Work Zero