just trying to modify the m6 to move x to home position for toolchange

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
playerofpawns1
Posts: 1
Joined: Thu Jan 13, 2022 4:56 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: E062347D88BB-0505214750

just trying to modify the m6 to move x to home position for toolchange

Post by playerofpawns1 »

I am having problems being able to get a tool in when the spindle is sitting right above the part and the tool is long. I wish the x would move to home after z moves to home so I could get the spindle away from the part, can anyone help me get that set up. I'm sure it's simple to get that updated. thanks for your help in advance.
Attachments
report_E062347D88BB-0505214750_2022-01-13_12-34-41.zip
my report.
(687.1 KiB) Downloaded 3 times
ShawnM
Posts: 760
Joined: Fri May 24, 2019 8:34 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 7804734C6498-0401191832
Location: Clearwater, FL

Re: just trying to modify the m6 to move x to home position for toolchange

Post by ShawnM »

Deleted - I was confused as to what he was asking.
Last edited by ShawnM on Fri Jan 14, 2022 1:28 am, edited 1 time in total.
cncsnw
Posts: 2424
Joined: Wed Mar 24, 2010 5:48 pm

Re: just trying to modify the m6 to move x to home position for toolchange

Post by cncsnw »

The order of power-up homing that you set in the Wizard has nothing to do with axis movement during tool changes.

Macro functions that you assign to Aux keys are not operable while a program cycle is running, and so are not useful at a tool-change prompt within a program.

You need to create a new file in the c:\cncm directory, named "mfunc6.mac". You could make it read something like this:

Code: Select all

; M6 - tool change
G91 G28 X0  ; move X axis to return point #1
G90         ; restore absolute positioning mode
M6          ; do default M6 action (prompt for tool and wait for cycle start)
ShawnM
Posts: 760
Joined: Fri May 24, 2019 8:34 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 7804734C6498-0401191832
Location: Clearwater, FL

Re: just trying to modify the m6 to move x to home position for toolchange

Post by ShawnM »

I see what he's asking now, he's trying to do a tool change over the part during a job after the Z axis moves up but there's no X or Y movement afterwards. My bad. Yes, just modify the M6 macro to move the spindle to your designated tool change position for easy access. Thanks for opening my eyes cncsnw.
tblough
Posts: 1874
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
Location: Boston, MA
Contact:

Re: just trying to modify the m6 to move x to home position for toolchange

Post by tblough »

Your other option is to hit escape to exit the program, jog the machine where you need it for the toolchange, change your tool, and then hit F4 Run/F1 Resume.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
Gary Campbell
Posts: 1702
Joined: Sat Nov 18, 2017 2:32 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: Acorn 238
Location: Marquette, MI
Contact:

Re: just trying to modify the m6 to move x to home position for toolchange

Post by Gary Campbell »

Set your G28 Position (or any of the 4 returns) to your desired toolchange location
Edit your mfunc6.mac and add "G28" in the line after the "M5" command
GCnC Control
CNC Control & Retrofits
https://www.youtube.com/user/Islaww1/videos
martyscncgarage
Posts: 9474
Joined: Tue Mar 28, 2017 12:01 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: Yes
CPU10 or CPU7: Yes
CNC Control System Serial Number: none
Location: Mesa, AZ

Re: just trying to modify the m6 to move x to home position for toolchange

Post by martyscncgarage »

playerofpawns1 wrote: Thu Jan 13, 2022 5:01 pm I am having problems being able to get a tool in when the spindle is sitting right above the part and the tool is long. I wish the x would move to home after z moves to home so I could get the spindle away from the part, can anyone help me get that set up. I'm sure it's simple to get that updated. thanks for your help in advance.
You've been given good advice. Let us know what you ended up doing.
The key as I see it is the part/fixture going to be different often enough that you can not automate the tool change? If so, you will have to move the machine manually during the tool change as was suggested.

Creating and customizing the mfunc6.mac would be the way to go otherwise.
Both Marc (cncsnw) and Gary suggested using G28 or one of the others to set the tool change position and add it to your Mfunc6.mac

Let us know how you make out. Post a fresh report after you have accomplished the task.
Marty
Reminder, for support please follow this post: viewtopic.php?f=20&t=383
We can't "SEE" what you see...
Mesa, AZ
Muzzer
Posts: 534
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: just trying to modify the m6 to move x to home position for toolchange

Post by Muzzer »

I didn't see what CAM program is being used here but if you are using Fusion 360, the post processor inserts a "safe retract" ahead of a manual tool change. In the case of Centroid, the post processor dialog options for safe retract are G28, G30, G30 P3, G30 P4 or simply "clearance height".

You can define the X, Y & Z coordinates for the G30 retracts in CNC12 if desired. No need to play with mfunc6.

On my machine I simply do a G28 which is like a "tool check", as I can easily grab the toolholder without moving the table in X & Y.
Post Reply