need a basic m6 start macro
If anyone could help I need a basic MANUAL tool change macro. I sometimes have 10 tool changes on a single set up and would like to be able to use a macro instead of 10 single programs .
I would like to have it G53 -4" (from Zhome limit(
Ask for tool change with message
change T#@m6 command
Change H#@43 command
Drive back down to last retract in program prior to the tool change .
If anyone could help out that would be great . I found a couple but they don't seem to work for me.
Re: need a basic m6 start macro
I have several older machines using fanuc, closest are 10M control's.
Depending on the parameter setup, I have never needed G53. However I understand it's importance. I refer you here... G28 Versus G53 : Modern Machine Shop
this simple macro works for me, again 10M fanuc with tweaked parameters.
%
O9001(TOOL CHANGE MACRO)
M09
M05
G0G94G40G90G80G28G49Z0
G91G30
M6
G0G90
M99
%
I know, each machine has it's quirks.
Re: need a basic m6 start macro
Quote:
Originally Posted by
LEARN
no G28 will work I was just trying to keep z down a bit so I can change tools easier lol. I will try that 1 out . Thanks
Keep Z down a bit? lol, i'm confused. Tool changer messed up? I often don't see things so...
Yeah, I'm lost, lol.
Re: need a basic m6 start macro
There is a good one I found on YouTube.
I will post the link up later tonight.
Its simple and works very well, I did have to add the tool offset to it if I recall correctly. The macro will go to the specified z height for the tool change, default was -1 from home pos I think, it will display a message asking for you to put in tool # "...". When you have changed out to the new tool, you press "ok" and it will lower to 0.25" above the part surface and then begin to machine.
Re: need a basic m6 start macro
What you're asking for would be better handled by your post processor, as you're not doing anything that really requires the M6Start macro.
Quote:
I would like to have it G53 -4" (from Zhome limit(
This is a simple "G53 G0 Zxx" move
Quote:
Ask for tool change with message
change T#@m6 command
All you need is a T# M6 in your g-code, and Mach3 will stop and wait for you to press Cycle Start to continue.
Quote:
Change H#@43 command
You're next line of g-code should be G43 H#
Quote:
Drive back down to last retract in program prior to the tool change .
Just add another line of g-code to move to where it was. This may be the only tricky part.
Re: need a basic m6 start macro
The M6 on that fanuc does many things as well as stopping the spindle, coolant, moving head to tool change position, I use the macro to additionally add a few tweaks I may use daily without having to think about them. I am still confused as to how your using them.
off the top of my head:
O0013;
T1 M6;
N1 M1;
G56 X0 Y0 S1250 M3;
G43 H1 Z1. M8;
G81 Z-.06 R.05 F1.;
G80 M9;
T2 M6;
N2 M1;
etc...
Simple spotting cycle.
Hope i'm helping
Re: need a basic m6 start macro
https://www.youtube.com/watch?v=D_XlXBq2Szs
M6 Start Macro
'Tool Change Macro For Manual tool change 09/14 CNC4XR7
OldTool = GetOEMDRO (1224) 'Tool In spindle DRO You must add this to your settings screen
'x = GetToolChangeStart( 0 ) ' Get x tool change start position
'y = GetToolChangeStart( 1 ) ' Get y tool change start position
'z = GetToolChangeStart( 2 ) ' Get z tool change start position
Code "G53 G0 Z-2.0" ' Move z to tool change position in Machine cord.
While IsMoving ' wait for z to move
Wend
tool = GetSelectedTool() ' tool to be changed to
NewTool = tool
Call SetUserDRO (1224,NewTool)
SetCurrentTool( NewTool ) ' input new tool into tool in spindle dro
Code "G43 H" & tool ' Call tool offsets for new tool
' Verify Tool Change Complete
Dim Msg, Style, Title, Help, Ctxt, Response,MyString
Msg = "Please Insert Tool Number " & " ( " & GetSelectedTool() & " ) " & " " & GetToolDesc(tool) ' Define message
Style = vbYesNo + vbCritical + vbDefaultButton2 ' Define buttons
Style = 0 + 48 + 0 ' Define buttons.
Title = "Tool Change Requested" ' Define title
Help = "DEMO.HLP" ' Define Help file
Ctxt = 1000 ' Define topic 'context. ' Display message.
Response = MsgBox(Msg, Style, Title, Help, Ctxt)
If Response = vbOk Then ' User chose Ok
MyString = "Ok" ' Perform some action
End If
Message "Tool # " & GetCurrentTool() & " : " & GetToolDesc(GetCurrentTool()) & " Installed " & " Returning to Tool Change Start Position"
'Code "G00 X" & x & "Y" & y & "Z" & z 'Move back to where the tool change was prompted
Code "G00 Z .25" 'Move Z back to .25" above zero in work cord.
While IsMoving
Wend
End
Re: need a basic m6 start macro
NOT related to this thread. No trolling intended.
THAT'S A LITTLE TOY!
Ignore me, I know how stressful this can be.
lol
Re: need a basic m6 start macro
It worked but when you actually tried to use it it did not start cutting? Could you elaborate a little more. It's been working great for a month for me now. You can also modify it, it's pretty easy so see what control what once it's laid out
Re: need a basic m6 start macro
OH! manual tool change? That makes things clearer (is clearer a word?) G28 versus G53, ok, let me get some info, i just researched this a short time ago. G28 Versus G53 : Modern Machine Shop
This guy is scary smart.
I hope i'm helping.
Re: need a basic m6 start macro
Quote:
Originally Posted by
Alax7
It worked but when you actually tried to use it it did not start cutting? Could you elaborate a little more. It's been working great for a month for me now. You can also modify it, it's pretty easy so see what control what once it's laid out
I will have to try it again as soon as the weather gets better and report back. I had tried 2 different modifications of this macro.
The first macro I can recall exactly what was wrong but I know it was not correct.
the 2nd macro would drive up in Z to the G53 z-100. position . then ask for tool change only making it to the M6 T1 command. At that point it did not change the T# in the DRO . After that it would drive down above the work piece then back up to the G53 position asking for the tool change again
- - - Updated - - -
It would be nice to see some other examples of other peoples MANUAL tool change m6 macros. I am sure many of you use them
Re: need a basic m6 start macro
After doing a bunch of searches on google (lol of all places ) I found a link that led to CNC ZONE haha and I found a basic tool change that does work ( at least on my lap top still to cold to go out to the garage )
tool = GetSelectedTool()
SetCurrentTool( tool )
Code "G53 G0 Z0"
While IsMoving
Wend
Code "G53 G0 X0 Y0"
While IsMoving
Wend
IT was posted by the MOD here " ger21 " Thanks
Re: need a basic m6 start macro
Well done. I assigned M7 (as I don't have this oil shot function) to a basic G53 G92 macro that works very well in cycle. Nice to know a little extra, isn't it? lol
Re: need a basic m6 start macro
What does the M7 do ?
I have a manual oiler as well
Re: need a basic m6 start macro
Quote:
G28 Versus G53 : Modern Machine Shop
From the above:
"This means you may have machines that do not allow G53 (without purchasing G53 from FANUC)."
I find this almost incredible. Does this mean you have to BUY the (ability to execute) G53 instruction from Fanuc for their controller?????????
The mind boggles!
Cheers
Roger