Hello Guest it is March 05, 2021, 05:10:52 AM

Author Topic: setting the exact home for 2 different files  (Read 186 times)

0 Members and 1 Guest are viewing this topic.

setting the exact home for 2 different files
« on: July 21, 2020, 01:43:55 PM »
Hello, I am trying to cut 1" PVC Letters however I need to drill specific holes on the back only 1/2" down. if I have 2 separate files(one for the holes the other for the through cut) how do i set the home in Mach3 in the same exact position for both files. Have to use 2 different size bits that's why 2 files.
(unless someone knows how to do a bit change mid job and have the Z axis stay the same because I can just use 1 file if that's the case.)
still fairly new to this and was thrown to the wolves.
any help is appreciated.
email-eseager1114@gmail.com
THANK YOU

Offline JG

*
  •  50 50
    • View Profile
Re: setting the exact home for 2 different files
« Reply #1 on: July 21, 2020, 02:25:46 PM »
I'm also very new to Mach3 and CNC but I think that adding  M6  where you need to change the tool will wait for you to do so and then click on [ Start ] again once you've done so.


Someone with more knowledge will no doubt confirm or deny my assertion  :)

Offline Graham Waterworth

*
  • *
  •  2,275 2,275
  • Yorkshire Dales, England
    • View Profile
Re: setting the exact home for 2 different files
« Reply #2 on: July 21, 2020, 07:23:33 PM »
Touch the first tool on the top face of the job.

Click Zero Z button.

Then enter 1 in the 'Tool' DRO in the Tool Information box.

Then enter its diameter in the Dia DRO

Followed by the length, set this to zero

Put the second tool in the spindle.

Touch it on the top of the job

Then enter 2 in the 'Tool' DRO in the Tool Information box.

Then its diameter in the Dia DRO

Then set the length to the value shown in the Z axis DRO, this is the difference in length between tool 1 and tool 2, so tool 2 has and offset in length that Mach3 compensates for.

-----------

Your first program should have G43 H1 on the first Z rapid line

The second program should have G43 H2

e.g.

O0001 (FIRST PROGRAM)

G21 G40 G00 G99 G17

G54 G00 G90 G43 X0 Y0
G43 H1 Z10.
S1000 M3
etc...
M30

O0002 (2ND PROGRAM)

G21 G40 G00 G99 G17

G54 G00 G90 G43 X0 Y0
G43 H2 Z10.
S1000 M3
etc...
M30

Or you could join the 2 programs together.

O0001 (FIRST & 2ND PROGRAM)

G21 G40 G00 G99 G17

N1 (TOOL 1)
G54 G00 G90 G43 X0 Y0
G43 H1 Z10.
S1000 M3
etc...
M0

(CHANGE TO 2ND TOOL)

N2 (TOOL 2)
G54 G00 G90 G43 X0 Y0
G43 H2 Z10.
S1000 M3
etc...
M30

You can also use the Offset screen to set tools, bottom right of screen
Without engineers the world stops