Hello Guest it is February 26, 2021, 05:49:05 AM

Author Topic: Not getting how to use tool length offsets  (Read 13346 times)

0 Members and 1 Guest are viewing this topic.

Not getting how to use tool length offsets
« on: July 23, 2013, 09:14:59 PM »
I've used tool length offsets extensively in the past on a Fadal and also an old Bandit controller.  However I am just not getting it with Mach 3!  I crashed a drill into a part destroying it after I thought I understood from a test run. What I wanted to do was use my edge finder as a touch off tool to find edges and the top of a part.  So I was going to call that tool zero and always leave it setup.  I have tool height setter with an LED and 0.200 overtravel that is 2" tall. So I was going to pick a spot on the table and always place it there. Once all the tools are set on the presetter I should be able to pick up the sides and top of the part in the fixture using tool zero and set all axes to zero. Then tool changes that call tools 1 and up should get positioned correctly.

Issues that I see:

I see where there is a tool change position X=0 Y=0 Z=5", but a tool change called in g-code from Cambam does not move to a tool change position.  The move appears to be enabled on the settings page. What else controls this?  What code makes it do the move? Does the tool length offset get applied first after the tool change, moving the Z so the tip of the new tool is at 5"? I think if the machine doesn't move to the tool change  position then everything else pretty much fails.

Thanks,

Gary H. Lucas
Re: Not getting how to use tool length offsets
« Reply #1 on: July 24, 2013, 03:55:32 AM »
In g-code you need to call height offset using G43 H(offset number from mach tool table).
Offset is taken account in next z move. Be carefull to have enough space from tool change location and next move, it must be more than offset value.

Personaly I do not use any special macro to send machine to the tool change location, I just edit M6 start macro and use machine coordinates to sent machine tool change location. This way machine will move to the tool change location allways when program have M6 in it.

My M6 macro I have:
G0 G53 Z0 ( z to machine zero )

Cam just outputs:
...
M6 T2
S4500 M3
G43 H2
G0 Z2.
...
Re: Not getting how to use tool length offsets
« Reply #2 on: August 07, 2013, 10:51:24 PM »
I did a tool change script in Mach 3

The tread is here: http://www.cambam.co.uk/forum/index.php?topic=2044.0

Script:
A poster on the CNCZone helped me refine the script for the M6start file.
This will get the Tool Change Postions in the Mach3 settings and move to
that position for the tool change then move back.

I have not fully tested it but it seems to work great.


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
Re: Not getting how to use tool length offsets
« Reply #3 on: August 07, 2013, 10:54:13 PM »
I edited my Mach screen set to add a set tool change location button as well.

All I do is jog to the desired tool change location, hit the "set tool change location" button on the screen and go.

I use tool #1 as my tool setting spot
Re: Not getting how to use tool length offsets
« Reply #4 on: August 23, 2013, 01:30:18 PM »
Looks like you have received some good helpful responses but I will add if you had a crash while using TLO's the two most common culprits are not calling G43 Hx, or being in a different work offset than where you set your Z zero.  Personally I don't use a tool change location either, on my Tormach it happens wherever you are, very convenient.  For measuring and setting tool length offsets I reserve a work offset such as G58, when it's time to set TLO's I just call G58 G0 X0 Y0, making sure you have adequate Z height.  Most measuring routines will call G49 since you are measuring an absolute length, so you will loose your G43 call.  As a safety if you call the work offset such as G54, and call G43 Hx in your G code part program you'll go along way in avoiding any more nasty noises.

Are you hand entering the tool lengths in the tool table?  This is another potential for fat-fingered errors.  If you are, you may want to check out CNCneeds automatic tool setter, very accurate, very affordable, it's compatible with Tormach's Automatic Tool Changer touch-off routine, and best of all it enters the data directly in the tool table as it measures each tool.
http://www.cncneeds.com/index.html