[extsuba]

Hello
I am running a cnc knee mill with mach3 tied to dugong drives and cnc drive breakout board hooked into smooth stepper. I am having a problem trying to get mach3 to go to machine zero for a tool change, I do have the following:
Tool library - nmtb30 holder
Homing and limit switches
Every time the mill is powered on the machine is referenced
machine stops for tool changes under general settings
and optional stops m codes are enabled


I have seen the option of editing the start and end macros but no clue on what to put there

I did try to put in the location in the settings area under tool change
but no luck

I would like this to be in the controller side
and not program a location in each part program - it was suggested as a solution on another forum

Thank you for the help

[HelicopterJohn]

Hi,

I use the Mach3 2010 Screen Set with my Shopbot CNC Router with USB Smooth Stepper. It will allow you to do Semi-Automatic Tool Changes and also define a Tool Change Position.

I don't know if that screenset would work on your machine or not but you could contact GER21 for addtional details.

The CNC Woodworker - Mach3 2010

John

[ger21]

The default M6Start macro is this:

tool = GetSelectedTool()
SetCurrentTool( tool )

If you want to move to machine zero, change it to this:

tool = GetSelectedTool()
SetCurrentTool( tool )
Code "G53 G0 Z0"
While IsMoving
Wend
Code "G53 G0 X0 Y0"
While IsMoving
Wend


Make sure that Z zero in machine coordinates is the top of your travel, or at least some distance up that is safe to move at.

[extsuba]

IT worked like a charm - Thanks - What else can this file do

[adprinter]

The default M6Start macro is this:

tool = GetSelectedTool()
SetCurrentTool( tool )

If you want to move to machine zero, change it to this:

tool = GetSelectedTool()
SetCurrentTool( tool )
Code "G53 G0 Z0"
While IsMoving
Wend
Code "G53 G0 X0 Y0"
While IsMoving
Wend


Make sure that Z zero in machine coordinates is the top of your travel, or at least some distance up that is safe to move at.

Ger, I too am trying to set up Mach3 to go to a fixed location (Machine Coordinates) for tool changes. Is it necessary to add the DoStopSpin() after the tool=GetSelectedTool() SetCurrentTool(tool)? Or will Mach3 automatically stop the spindle when it reads an M6 in the Gcode? Also, I have read that the Autotoolchanger option should be checked in the General configuration settings, in order for the M6 macro to move to a tool change position. I set up the Tool Change Position coordinates in the Mach3 Settings screen, and selected the Autotoolchanger option in the General configuration screen, and then tested it with just a simple Gcode which included two tool changes. (Just to test things out, and see if Mach3 would move the router to the machine coordinates entered in the Tool Change Position on the Settings screen). It did NOT! In fact, (since Autotoolchanger was selected), all that occurred, was the spindle stopped, (for the dwell setting of 2 seconds) then restarted. I don't actually HAVE an Automatic tool changer. But am hoping to set up Mach3, to do the following things (anytime an M6 is encountered in the Gcode file running):
1-Save the current coordinates
2-Stop the Spindle rotation
3-Move to the desired Machine Coordinates of Z=0 X=27 Y=7
4-WAIT for ME to change the tool, and reset the Z zero work coordinate (touch off)
5-Start the Spindle rotation
6-Return the router to the saved coordinates
7-Continue executing the current G code file
So, my question is this:
Should I set the Tool change option in the General Configuration Screen back to "Stop Spindle, wait for tool change", and just alter the M6Start macro to the following:
tool = GetSelectedTool()
SetCurrentTool( tool )
DoSpinStop()
Code "G53 G0 Z0"
While IsMoving
Wend
Code "G53 G0 X27 Y7"
While IsMoving
Wend

Or should the DoSpinStop() be omitted? I am not at all familiar with Visual BASIC and am just starting to learn. And it is confusing, since the Spindle does stop rotating when the M6 is encountered in the G code. I am assuming that this is an automatic function in Mach3, since it does not appear to be commanded in the M6Start default macro. My apologies to the Original Poster of this thread, it was not my intention to hijack..... just seeking an answer from those who know.

[ger21]

There are a lot of questions in your post.

If you set Mach3 to Automatic Toolchange mode, it will run the M6 start macro, and then continue on. That's not what you want.

As you guessed, you want "Stop spindle, wait for Cycle Start." As it says, it will stop the spindle, so you don't need the DoSpinStop().
However, it's a good idea to always have an M5 in your g-code prior to the M6 to stop the spindle before the macro.

The M6 Start should be modified the way you have it.
Once the M6 start is finished, Mach3 will wait for you to press Cycle Start. This is when you'll change the tool.

Once you press Cycle Start, Mach3 will then run the M6End macro. This is where you'll return to the previous position.
My recommendation is to have the G code start the spindle rather than the macro.

Have your g-code something like this:
M5
T2 M6
S10000 M3

This will:
Stop the spindle.
Call the toolchange
Set the rpm and start the spindle.

Also, unless you have pre-measured all your tools and are using G43 length offsets, you're going to need to zero the new tool before you continue.

[adprinter]

There are a lot of questions in your post.

If you set Mach3 to Automatic Toolchange mode, it will run the M6 start macro, and then continue on. That's not what you want.

As you guessed, you want "Stop spindle, wait for Cycle Start." As it says, it will stop the spindle, so you don't need the DoSpinStop().
However, it's a good idea to always have an M5 in your g-code prior to the M6 to stop the spindle before the macro.

The M6 Start should be modified the way you have it.
Once the M6 start is finished, Mach3 will wait for you to press Cycle Start. This is when you'll change the tool.

Once you press Cycle Start, Mach3 will then run the M6End macro. This is where you'll return to the previous position.
My recommendation is to have the G code start the spindle rather than the macro.

Have your g-code something like this:
M5
T2 M6
S10000 M3

This will:
Stop the spindle.
Call the toolchange
Set the rpm and start the spindle.

Also, unless you have pre-measured all your tools and are using G43 length offsets, you're going to need to zero the new tool before you continue.

Thanks, Gerry. I am aware of the need to re-zero the new tool during a tool change, and have been doing that for years. I really want to try out the 2010 screen set (and autozero macros) but quite honestly can't afford to pay the registration fee (or anything else these days) since I was forced to take an early retirement. So, what I was after, was to speed up tool changes as much as possible. Since the first thing I always have to do, is switch to the MDI screen in Mach3, and jog the machine to a comfortable position I can reach, change the tool, touch off the new tool, reset the Z zero, then press Cycle Start. By altering the M6Start macro, at least SOME of this process is automated. (It will move to the "Comfortable" position I can reach, and wait for me to change the tool). Again, THANKS for your help!

[Vegabond]

Hello guys!

I see this thread is old, but i have a problem..
I get error about the initial plane.. (see the attached picture)

How can i get rid of that??

Thanks!

Greetings from Robert.

[ger21]

Set the Clearance Plane to a value greater than 0, like it's telling you.

[Vegabond]

Here is the code.. and it seems not to be that problem?

N1 G21 G90
N2 (Top)
N3 G90
N4 T01 M06 (10.0 MM DIA MULTI-FLUTE END MILL)
N5 S10000 M3
N6 G0 X-5.003 Y10.46
N7 G43 H01 M8
N8 Z4 F1500.0
N9 G1 Z-20
N10 X-5
N11 Y139.523
N12 G0 Z5
N13 G90
N14
N15 G54
N16 M9
N17 M30
%

[ger21]

No, it's a setting on the screen somewhere.

[Vegabond]

Yes, but where!?

I have spent 5 hours here now... some other things i can try?