Machsupport Forum

G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: PhillM on April 28, 2013, 11:19:41 PM

Title: Simple M6 Manual Tool Change
Post by: PhillM on April 28, 2013, 11:19:41 PM
Hi ,

As i am pretty Green with all the CNC and the learning process is in progress I have been doing some simple drawings and GCode in cambam but I am a bit stuck on how to program in a tool change . At present I just want the machine to go to a XYZ cord which I will have to stop the spindle manually as I have not put in the auto control board as yet .

Then do a zero on the new tool and go back and continue the job , after re- zero on the tool.

I take it by changing the tool in CamBam this will automatically set the command for a M6 tool change in Mach3?
Title: Re: Simple M6 Manual Tool Change
Post by: Chaoticone on April 29, 2013, 09:57:21 AM
Yes, your cam program should print the M6, T***, etc.etc.  What you will need to do is work on your M6 macros if you want it to go to a certain position, stop, touch off, etc.

Brett
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 29, 2013, 05:54:25 PM
Hi Brett,

I have done and am learning  CamBam drawings but do find it easier to draw in profiler  anyway Ive put in different tools so I see in the gcode where each operation gives the M6 command .

 I am not up with is, where to and how to write in the M6 tool change , do a Z reset and then resume ...

You put in M6 tool change into the search and it is just full of a hole lot about Auto tool changers .
Title: Re: Simple M6 Manual Tool Change
Post by: Chaoticone on April 29, 2013, 08:17:48 PM
These 2 links will help you with your macros.

http://www.machsupport.com/wp-content/uploads/2013/02/Mach3_V3.x_Macro_Prog_Ref.pdf

http://www.machsupport.com/wp-content/uploads/2013/02/VBScript_Commands.pdf

Brett
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 29, 2013, 08:24:41 PM
I didn't realize there was a tutorial on tool change , but it still is leans heavily towards Auto tool changers but can see by changing some of the code it could be made to suit what I want , I downloaded the M6 Macros but there is nothing written to copy and paste except for this ,

This toolchanger macro is the example used in
the toolchanger video. It is not meant to be a fully working example
for your system, but rather one to be modified by the user.

Art

More than likely it is something I am doing ????

Thanks Brett , you posted while I was typing this , I will check your links out and try and get my head around it all
Title: Re: Simple M6 Manual Tool Change
Post by: ger21 on April 29, 2013, 10:19:01 PM
Go to General Config and set your Tool Change (upper left) to "Stop Spindle, Wait for Cycle Start".
Then go to the Settings page, and enter the tool change location (right side).

If you have a Tx M6 in your code, Mach3 should go to the tool change position and stop. You should then be able to change and rezero the new tool, and when you press Cycle Start, Mach3 will resume cutting.
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 29, 2013, 10:40:35 PM
Hi Gerry,

Thanks , I am a total novice in this field and trying to learn so please excuse me if I am asking dumb questions .

What if the tool change is asking for the same tool , how does it ignore that and keep cutting until a different tool is required .

As the " Tool Change Macro " Download does not appear to have any code I have had to print screen from the tutorial into paint and print the code which I am now manually typing into Note , and then try to modify to suit .

What I am trying to do is :

M6 Tool Change request ... Ignore if same tool ... Go to change position if tool New Tool is needed at safe height .... Then Do Manual Change and Re - Zero tool " .... enter new tool number  is stored either manually or changed to the tool requested number when cycle start is hit ...( If tool 0 is entered to ignore tool change) not really sure on that one .
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 30, 2013, 04:10:30 AM
Gerry ,

Put the settings in as you advised and ran a Cut program to see how it all works , the tools are all listed and it pulls up out of the job and waits for cycle start , displays the tool selected in the program. The only thing was it did not move to the specified tool change Coords entered into the Tool Change Position , I take it this is because the spindle is not being controlled by Mach3  .

Thanks for your help , I was hoping for the simple solution rather than having to read and study a F-18 manual to get the basics on how a plane flys .
Title: Re: Simple M6 Manual Tool Change
Post by: ger21 on April 30, 2013, 09:10:26 AM
I'll have to check the stock macros later today to see about moving to the tool change position. I thought they did, but I don't use them. You probably need to have SafeZ enabled, preferably set in Machine Coordinates.

AS for ignoring the TC if it's the same tool, that's bad g-code. If the tool isn't changing, there shouldn't be an M6 there. Either configure your CAM software to not output the M6 that isn't needed, or you'll need to modify the M6 macros to check the tool and ignore if it's the same as the current tool.
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 30, 2013, 06:26:28 PM
Thanks Gerry ,

I will look at the SafeZ settings today , and you would be right about the bad Gcode as that is a reflection of my skill level and putting the cuts in order to suit or deleting the M6 . As for reconfiguring Macros , I am not that savy with all the code lingo so I will be happy with just what can be easily set .

I have beeen wanting to get into CNC for some time and 6 weeks ago I decided to bite the bullet and build a Mill/ Router to learn on , and when I get to a better level of better competence with Mach3 and Cad then I will look at converting my bigger Mill .. Optium BF30 .  So to this point has been a pretty steep learning curve but I do have " phone a friend"  one being a CNC and  computer programmer but I try to work and find out as much as I can first 

I attached a pic of the Router , (http://) compared to what others have here its more of a toy .
Title: Re: Simple M6 Manual Tool Change
Post by: ger21 on April 30, 2013, 06:49:08 PM
I just took a look, and the stock macro's don't move to the tool change position. They do move back to the previous position after the tool change, though. The 2010 screenset that I sell  will move the tool to the toolchange position, and zero the tool for you automatically, in case you're interested. :)
Title: Re: Simple M6 Manual Tool Change
Post by: PhillM on April 30, 2013, 10:17:11 PM
Hi Gerry ,

Your Screen looks great , and has the manual tool change function that I was asking about , for the price you are asking I will be purchasing a copy and you seem to support your software with good tutorials for novices like me .. will be in contact soon .
Title: Re: Simple M6 Manual Tool Change
Post by: vithanidevesh on March 26, 2014, 04:20:32 AM
These 2 links will help you with your macros.

http://www.machsupport.com/docs/Mach3_V3.x_Macro_Prog_Ref.pdf

http://www.machsupport.com/docs/VBScript_Commands.pdf

Brett

Links not working??
Title: Re: Simple M6 Manual Tool Change
Post by: Chaoticone on March 26, 2014, 05:41:23 AM
No, all of the old links are broke now. I just updated the links in my earlier post.

Brett
Title: Re: Simple M6 Manual Tool Change
Post by: rstrohl56 on September 30, 2014, 05:28:16 PM
I am using Mach3 Turn to run an Emco Turn 50 Lathe. I would like to use CNCBase software to write code. The problem I am having is that Mach 3 wants a different format for tool changes than I am used to. If I enter M3 T3, it gives me an invalid tool selection (Tool 0). If I enter M6 T0303 or M6 T300, it works. Can anything be changed to make it use a standard tool number?
Title: Re: Simple M6 Manual Tool Change
Post by: Graham Waterworth on October 01, 2014, 05:19:08 PM
T0606 and the like is standard for turning T6 M6 is standard for mills and routers.

Title: Re: Simple M6 Manual Tool Change
Post by: voyager1972 on April 23, 2019, 05:53:10 AM
is there a macro available to get the "tool change location" option in mach3 to function,,,and goto x,y,z bed loaction when a tool change is requested .
Title: Re: Simple M6 Manual Tool Change
Post by: ZASto on April 23, 2019, 07:59:10 PM
On settings page there are three DROs for tool change location. They are in Machine Coordinates!!!
Machine should go to that location when Mach encounters M6 Tx.
Title: Re: Simple M6 Manual Tool Change
Post by: reuelt on April 26, 2019, 02:45:11 PM
is there a macro available to get the "tool change location" option in mach3 to function,,,and goto x,y,z bed location when a tool change is requested .

'You will need to edit m6Start.m1s macro (add the following lines there) to do that.

ToolChangeX = GetUserDRO(1200)            'Get user defined tool change location
ToolChangeY = GetUserDRO(1201)
ToolChangeZ = GetUserDRO(1202)   
     
If IsSafeZ() Then               'If SafeZ is defined,
   safeZ = GetSafeZ()            'use it for positioning commands
Else
   safeZ = 0               'Otherwise, moves are made at MC Z0
End If
Code" G53 G0 Z" & safeZ               'Position spindle for tool change
While IsMoving()
Wend
Code"G53 G0 X" & ToolChangeX & "Y" & ToolChangeY
While IsMoving()
Wend
Code"G53 G0 Z" & ToolChangeZ
While IsMoving()
Wend
Title: Re: Simple M6 Manual Tool Change
Post by: reuelt on April 26, 2019, 03:24:53 PM

'please add safez=0 to get it defined


ToolChangeX = GetUserDRO(1200)            'Get user defined tool change location
ToolChangeY = GetUserDRO(1201)
ToolChangeZ = GetUserDRO(1202)   
safeZ=0

If IsSafeZ() Then               'If SafeZ is defined,
   safeZ = GetSafeZ()            'use it for positioning commands
Else
   safeZ = 0               'Otherwise, moves are made at MC Z0
End If
Code" G53 G0 Z" & safeZ               'Position spindle for tool change
While IsMoving()
Wend
Code"G53 G0 X" & ToolChangeX & "Y" & ToolChangeY
While IsMoving()
Wend
Code"G53 G0 Z" & ToolChangeZ
While IsMoving()
Wend
Title: Re: Simple M6 Manual Tool Change
Post by: Olavi on July 24, 2020, 02:51:04 PM
Hi Gerry,

Thanks , I am a total novice in this field and trying to learn so please excuse me if I am asking dumb questions .

What if the tool change is asking for the same tool , how does it ignore that and keep cutting until a different tool is required .

As the " Tool Change Macro " Download does not appear to have any code I have had to print screen from the tutorial into paint and print the code which I am now manually typing into Note , and then try to modify to suit .

What I am trying to do is :

M6 Tool Change request ... Ignore if same tool ... Go to change position if tool New Tool is needed at safe height .... Then Do Manual Change and Re - Zero tool " .... enter new tool number  is stored either manually or changed to the tool requested number when cycle start is hit ...( If tool 0 is entered to ignore tool change) not really sure on that one .

I have same question - why Mach3 tries to change tool when required tool is already installed?

I know I can disable M6 at the beginning of job, but I dont want to do that. Is it possible to configure mach to change tool at the begin of job when it is needed only? At moment there are pretty useless movements before job can start. Also my CAD program (Aspire) cant know which tool may be used, so it will add that codeline just in case.
Title: Re: Simple M6 Manual Tool Change
Post by: ZASto on July 24, 2020, 05:47:17 PM
In your CAM program you can assign the tool number for every tool that you use.
In Mach3 EVERY M6 Tx will do a tool change routine even if the desired tool is loaded in your spindle.
A little of "useless" movements will not hurt you much, time wise.

It seems that people are too spoiled. When we had computers running DOS, from floppies, on 8086 processor, all was fine, nowadays, AMD Threadripper with ultrafast SSD is "slow" :D
Title: Re: Simple M6 Manual Tool Change
Post by: Olavi on July 25, 2020, 02:15:35 AM
It seems that people are too spoiled. When we had computers running DOS, from floppies, on 8086 processor, all was fine, nowadays, AMD Threadripper with ultrafast SSD is "slow" :D
ZASto is so spoiled. When my grandmom was young, she delivered letters around country with horses and everybody was happy. Nowadays ppl are not happy when getting so many emails. :D

Its not very big deal, I can skip any movements when tool is already loaded, just hitting cycle start twice. I personally think it is a bit strange why not to skip it. But it is ok.

Does same thing happen when using auto tool changer? CNC drops tool and reloads it?
Title: Re: Simple M6 Manual Tool Change
Post by: ZASto on July 25, 2020, 04:57:49 AM
You should then change M6start macro, through which you can skip all unnecessary movements if loaded tool is the same as commanded tool.
Title: Re: Simple M6 Manual Tool Change
Post by: Olavi on July 25, 2020, 05:02:11 AM
You should then change M6start macro, through which you can skip all unnecessary movements if loaded tool is the same as commanded tool.
You have right.

Also I am looking for mach4 which skips tool change when it is not needed.

Ty for your answers, ZASto. :)
Title: Re: Simple M6 Manual Tool Change
Post by: Olavi on July 31, 2020, 07:25:24 PM
I found out that Mach3 dont try to change existing tool when using auto tool changer (instead of stop spindle option). So I am making script by this way.