How do I do a manual tool change?

17 Nov 2013 22:17 - 17 Nov 2013 23:10 #40893 by ArcEye

I will be able to test your config later, but I suspect I have found the problem.

# loadusr -W hal_manualtoolchange
loadusr -W hal_manualtoolchange_jog

net tool-change iocontrol.0.tool-change => hal_manualtoolchange.change
net tool-changed iocontrol.0.tool-changed <= hal_manualtoolchange.changed
net tool-number iocontrol.0.tool-prep-number => hal_manualtoolchange.number
net tool-prepare-loopback iocontrol.0.tool-prepare => iocontrol.0.tool-prepared

You have renamed the component file to hal_manualtoolchange_jog

Unless you have edited the component code to rename the component to the same name,
it will launch the component which is still called hal_manualtoolchange and wait for ever for a component called hal_manualtoolchange_jog to become ready, which it never will.

Then it would error anyway because iocontrol is still linked to hal_manualtoolchange

Revert to the original name and it should work

Last Edit: 17 Nov 2013 23:10 by ArcEye.
17 Nov 2013 23:09 #40897 by ArcEye
Yep, that is exactly what is wrong with it

Changed it back to original name and

18 Nov 2013 00:14 #40900 by LS
Great thank you! I just tested it, and it's working for me too.

I'd spent plenty of time looking at the code, but never would have thought about the filename.

This will make life easier to be able to jog during manual tool changes.

20 Jan 2014 22:40 #43029 by eslavko

Till now I use the old branded machine. (EMC2 - it's works so I didn't change)
But now I make another one for a friend. And component doesn't work as should.

When M6 is executed the popup window is shown. And I happily change tool and make Z touchoff.
When I press continue tha machine start immediatly with spindle OFF!

So how to add spindle on and to wait spindle-at-speed signal (my spindle make slow ramping to reach speed)
Of course I can start spindle manualy after changing and wait enought to startup before click continue..
...but preffer automatic!.
20 Jan 2014 23:47 #43030 by ArcEye

I just do it in G Code if I want the spindle stopped and re-started

G4 P10

There are so many different types of toolchanger, with a lot not wanting the spindle stopped (almost all lathes), coding it is probably easiest

20 Jan 2014 23:54 #43031 by eslavko

ArcEye wrote: ...
G4 P10

Maybe this is good option as in most cases when tool is changed the spindle speed is changed too.
25 Oct 2016 22:18 #82065 by robksawyer
I know this is a pretty old post, but I'm having the same issues as you were Gold Boarder. Can you share your latest config files? I'm also curious to see how you setup the Auto, Manual and MDI HAL GUI. Thanks.
25 Oct 2016 22:29 #82067 by andypugh
(User names are above the avatar, "Gold Boarder" is just a sign that he has posted a few hundred messages.)

Can you describe exactly what problems you are having?
25 Oct 2016 22:36 - 25 Oct 2016 22:37 #82068 by robksawyer
Ha (noob), realized that shortly after posting. I'm trying to get to where @eslavko is at (see below). I'm having the issue where linuxcnc is not letting me control the machine during this process. Also, I'm wondering if I should be going back to G53 (my home position) before the tool change instead of currently just raising the Z axis. I'm not sure how to do this exactly. Should I just run N90 G53 with no other parameters? I've attached an example of my current code.

"When M6 is executed the popup window is shown. And I happily change tool and make Z touchoff."

Machine: Sherline 5400 Mill
(T1  D=0.1275 CR=0. - ZMIN=-0.02 - FLAT END MILL)
(T50  D=0.0591 CR=0. - ZMIN=-0.002 - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z1.5
(18 TRACE1 0.02 OFFSET)
N25 T1 M6
N30 G0 X-1.0625 Y0.5413 Z0.6
N35 Z0.2
N40 G1 Z-0.02 F10.
N45 X-1.375 Y0. F20.
N50 X-1.0625 Y-0.5413
N55 X-0.4375
N60 X-0.125 Y0.
N65 X-0.4375 Y0.5413
N70 X-1.0625
N75 Z0.2 F10.
N80 G0 Z0.6
N90 G53 Z1.5
(1.5MM TRACE 0.002 OFFSET)
N95 M1
N100 T50 M6
N105 G0 X0.5485 Y-0.5413 Z0.6
N110 Z0.2
N115 G1 Z-0.002 F3.937
N120 X1.1735 F5.906
N125 X1.486 Y0.
N130 X1.1735 Y0.5413
N135 X0.5485
N140 X0.236 Y0.
N145 X0.5485 Y-0.5413
N150 Z0.2 F3.937
N155 G0 Z0.6
N165 G53 Z1.5
N170 M30
Last Edit: 25 Oct 2016 22:37 by robksawyer.
26 Oct 2016 14:03 #82085 by agris
Hi, robksawyer

It's been mentioned above - you need to change hal_manualtoolchange file (located at /usr/bin)
it's a Python script LinuxCNC calls when M6 command is issued.
My owm machine uses new hal_manualtoolchange (see attach) - it's a bit buggy with LinuxCNC 2.7 but works.

Your G53 question is pretty simple - you may add any code prior to toolchange in your postprocessor, or manually.
Just an example: raise Z, then move to machine coordinates X10 Y200. Do toolchange. Raise Z again to safe top.
... your actual milling code 
G0 G53 Z100
G0 G53 X10 Y200
M6 T5
G0 G53 Z100
... your actual milling code
Time to create page: 0.184 seconds
Powered by Kunena Forum