Need Help!- Help with mods to this Automatic Manual Tool Changer

[kregan]

Hi all,

Over the weekend I found and installed this script to work as a semi automatic tool changer
for use with the Tormach style tools in my small mill.

I would like some help on updating this to work with the UserDRO's in the offset's page
under "tool change location".

I am not sure how to do this?


Here is the existing script that was written for Mach2:

-------------------------------------------------

The M6Start.m1s file should contain the following

SafeZ=GetSafeZ() 'Load Safe Z Value
Code"G53 G00 Z" & SafeZ 'Goto the safe Z Location
Code"M99999" 'Call Macro M99999

Then make a new file called M99999.m1s with the following:

tool=GetSelectedTool() 'Load the tool number
SetCurrentTool(tool) 'Set the tool
Code "g43 H" & tool 'Set the height

Complete=Question ("Change to tool number" & tool

---------------------------------------------------

Possible new script...

M6Start.m1s file:

x = GetUserDRO( 1200 )
y = GetUserDRO( 1201 )
z = GetUserDRO( 1202 )

Code' G53G0 Z' & Z
Code' G53G0 X' & x & 'Y' & y
Code"M99999" 'Call Macro M99999


M99999.m1s file:

tool=GetSelectedTool() 'Load the tool number
SetCurrentTool(tool) 'Set the tool
Code "g43 H" & tool 'Set the height

Complete=Question ("Change to tool number" & tool

------------------------------------------------------

I don't know what to add to rapid back to the starting location?

Totaly new to scripts so don't laugh to hard if it is way off.

[ger21]

I do it something like this. I'm not moving back to the previous Z position, but you can see how to do it.

Also, I don't see the purpose of this line, and it appears to be missing a ).
Complete=Question ("Change to tool number" & tool

Try this. I actually store the tool change position in variables, as I use M6 End to retrieve the position and move there.

SetVar(1, GetOEMDRO(800))
SetVar(2, GetOEMDRO(801))
SetVar(3, GetOEMDRO(802))
TCX=GetOEMDRO(1200)
TCY=GetOEMDRO(1201)
TCZ=GetOEMDRO(1202)


Code "G53 G0 Z " & TCZ
While IsMoving
Wend
Code "G53 G0 X" & TCX & "Y" & TCY
While IsMoving
Wend
Code "M99999"
While IsMoving
Wend

Code "G0 X" & GetVar(1) & " Y" & GetVar(2) ' Move to Previous XY Position prior to M6 being called

While IsMoving()
Wend

[kregan]

Gerry,

That is awesome! Thank you!
I tried it out briefly tonight just moving in air and it seems to work perfectly.

One issue I get is a limit switch warning but I think that is due to the fact that this is a round column machine with the quil driven for the Z axis. I only have 4"
of travel and HOME shares the limit switch and it is all set very close.

I will do some test cutting and report back.

[kregan]

That was my typo...
The change tool number message appears in a box on the screen when a tool change is called for. It has another box next to it that requires me to type in the tool number I inserted into the machine and hit enter...

Originally Posted by ger21 I do it something like this. I'm not moving back to the previous Z position, but you can see how to do it. Also, I don't see the purpose of this line, and it appears to be missing a ). Complete=Question ("Change to tool number" & tool

[kregan]

I ran a bunch of parts today and the script worked perfectly.

Thank you again!

[kregan]

I know this is an old thread of mine but I have a question.

My new square column machine has more Z travel then my old round column and often my tool change position is a lot higher so it can take a while for the Z to move down into position.

If I want the machine to rapid back to the previous Z position do I change the code from this:

Code "G0 X" & GetVar(1) & " Y" & GetVar(2) ' Move to Previous XY Position prior to M6 being called

to this:

Code "G0 X" & GetVar(1) & " Y" & GetVar(2) & "Z" & GetVar(3) ' Move to Previous XYZ Position prior to M6 being called

Thank you for the help.

Originally Posted by ger21 I do it something like this. I'm not moving back to the previous Z position, but you can see how to do it. Also, I don't see the purpose of this line, and it appears to be missing a ). Complete=Question ("Change to tool number" & tool Try this. I actually store the tool change position in variables, as I use M6 End to retrieve the position and move there. SetVar(1, GetOEMDRO(800)) SetVar(2, GetOEMDRO(801)) SetVar(3, GetOEMDRO(802)) TCX=GetOEMDRO(1200) TCY=GetOEMDRO(1201) TCZ=GetOEMDRO(1202) Code "G53 G0 Z " & TCZ While IsMoving Wend Code "G53 G0 X" & TCX & "Y" & TCY While IsMoving Wend Code "M99999" While IsMoving Wend Code "G0 X" & GetVar(1) & " Y" & GetVar(2) ' Move to Previous XY Position prior to M6 being called While IsMoving() Wend

[ger21]

Yes, but sometimes it's safer to move the X and Y first, and then move the Z down.

[kregan]

Yes I would like to move X Y and then Z...
I am really clueless with the scrips so how would I do that?

Thank you.

Originally Posted by ger21 Yes, but sometimes it's safer to move the X and Y first, and then move the Z down.

[ger21]

Code "G0 X" & GetVar(1) & " Y" & GetVar(2) ' Move to Previous XY Position prior to M6 being called

Code "G0 Z" & GetVar(3) ' Move to Previous Z Position prior to M6 being called

[kregan]

Thank you very much for the quick help. I will test this out
and report back when I can.

Originally Posted by ger21 Code "G0 X" & GetVar(1) & " Y" & GetVar(2) ' Move to Previous XY Position prior to M6 being called Code "G0 Z" & GetVar(3) ' Move to Previous Z Position prior to M6 being called