Author Topic: Manual tool changes  (Read 945 times)

Offline Bob843

  • Ewok
  • *
  • Posts: 14
    • View Profile
Manual tool changes
« on: December 09, 2019, 22:59:41 pm »
Afternoon fellas my machine does not do auto tool changes can any one direct me to where i might find the g-code or how to program to stop the program raise the spindle so i can do a tool change then start right where program left off ?
 
Thanks Bob843
Urban Legend Customs

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6013
    • View Profile
    • Cambam V1.0 French Doc
Re: Manual tool changes
« Reply #1 on: December 10, 2019, 00:06:49 am »
Hello

First: your GCode must contain Tn M6 commands ; those commands are written by CamBam in the GCode when the tool number change between two machining operations (don't use 0 as tool number ; it disable toolchange)

ex: if the first mop use tool #4 and second mop with use tool #9, CamBam will write a T4 M6 before the first mop and a T9 M6 before the second mop ; if the tool number do not change between two mop, no Tn M6 will be written in the GCode.

So, you just need to take care that when a new tool is used for a machining operation, the tool number is different from the previous.

Be careful ; tools of different diameters must not share a same tool number ; if this is the case, CamBam will complain.

Second: The software that drive the machine must be set so it react to Tn M6 commands ... and it's software dependent ..

Ex, in Mach3 you can choose what the software must do when it encounter a Tn M6 (see picture)

- ignore toolchange

- stop and wait for manual toolchange.

- use an automatic toolchange macro (ATC)

after the tool has been changed, you must redo the Z 0 for the new tool.

What is you driving software ?

++
David
« Last Edit: December 10, 2019, 00:09:47 am by dh42 »

Offline driedeker

  • Storm Trooper
  • ***
  • Posts: 107
    • View Profile
« Last Edit: December 10, 2019, 07:09:47 am by driedeker »
Made in England in 53

Offline Bob843

  • Ewok
  • *
  • Posts: 14
    • View Profile
Re: Manual tool changes
« Reply #3 on: December 10, 2019, 15:55:13 pm »
yes i am using Mach 3 to run my machine
Urban Legend Customs

Offline Bob843

  • Ewok
  • *
  • Posts: 14
    • View Profile
Re: Manual tool changes
« Reply #4 on: December 10, 2019, 16:46:44 pm »
hello Dh42, it worked very well in a simulation after i made the changes in mach 3 outstanding thank you. now you guys got me looking at this mach 3 2010 LOL i cant seem to keep up with progress. thanks again men
Urban Legend Customs

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3943
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Manual tool changes
« Reply #5 on: December 11, 2019, 18:17:24 pm »
There are a number of different ways to manage manual tool changes on your machine. You can do it with the Tx tool number M6 and just have your machine stop. Mach3 unlike some other control software will allow you to jog the machine around and re zero the z after the tool change. you can use a tool change macro in Mac 3 to position the machine in a convenient location for the tool change, or you can do something similar in the post processor in cambam to insert code to move the machine to a convenient location for the tool change. If you're using path pilot or linuxcnc you may not be able to jog the machine around. I'm not 100% sure about a pure version of Linux CNC, but I know pathpilot which is a linuxcnc derivative does not allow you to jog the machine during a tool change. I do have my post processor for my pathpilot machine set to insert a g53 z0 f200 along with a tool change command. because that particular machine has tool holders that are pre measurable I use the tool table in the control software to set the length of every tool. I swap the tool and press start instead of having to jog and zero the tool. It really depends on what you have and how you want to tackle it. There are multiple possible solutions.
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 2937
    • View Profile
Re: Manual tool changes
« Reply #6 on: December 11, 2019, 20:24:08 pm »
If you use Mach 3, buy $20.00  mach3 2010 screen set, money well spend imho.
My 2ยข

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540

Offline Bob843

  • Ewok
  • *
  • Posts: 14
    • View Profile
Re: Manual tool changes
« Reply #7 on: December 12, 2019, 21:50:59 pm »
giving the mach3 2010 screen set some serious consideration, thanks to all who responded to my question
Urban Legend Customs

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4383
    • View Profile
Re: Manual tool changes
« Reply #8 on: December 13, 2019, 00:51:28 am »
I also use the 2010 screen set and can recommend it especially if easy tool changing and setting of Z zero is important to you.
Made in England