Acorn Tool Height offset problem
Moderator: cnckeith
-
- Posts: 17
- Joined: Mon Aug 24, 2020 6:18 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
Acorn Tool Height offset problem
Hello
I am hoping you can help me
I have a couple of problems:
Problem 1
I have a knee mill with a acorn cnc 12 retro fitted
it is 3 axis
i have p3 set to 0
So I have been following this vid:
So I set a reference tool
set height offsets for T1, T2 ,T3
I then set z depth using T2 and all is good. (T2 and H2 is displayed on the top right)
Now if I inset T3 (M6 T3) the tool number on the top right will change from T2 to T3 but the H2 still remains
is there a way that I can make it so the hight offset will always match the loaded tool?
Problem 2
When I do a tool change the z will move to the G28 position but not the xy position
I need it to move to the xyz position so it moves the job out of the way to give me space to remove the tool
I then made a m6 macro file and put in this:
M5
M9
G28
M6
This worked however every time i get an M6 it will move to this position
I think that there should be a way that it will skip the m6 if it has the correct tool in it all ready and run it if it hasn't got the right tool it in (then set the height off set at the same time)
is this possible?
For your information
I am using enroute to make my G code,
it is outputting a tool change like this:
N10 M25 G49 G17 G40
N20 T1 M6
N30 S2500 M3
N40 G0 X45. Y10. Z3.
N50 G1 Z-0.1 F200
N60 X80.
N70 Y80.
N80 X10.
N90 Y10.
N100 X45.
N110 G0 Z3.
N120 T2 M6
N130 S2500 M3
N140 G0 X45. Z3.
N150 G1 Z-0.1
N160 X90.
N170 Y90.
N180 X0.
N190 Y0.
N200 X45.
N210 G0 Z3.
N220 G40
N230 M5
N240 M9
N250 G80
N260 M30
I am hoping you can help me
I have a couple of problems:
Problem 1
I have a knee mill with a acorn cnc 12 retro fitted
it is 3 axis
i have p3 set to 0
So I have been following this vid:
So I set a reference tool
set height offsets for T1, T2 ,T3
I then set z depth using T2 and all is good. (T2 and H2 is displayed on the top right)
Now if I inset T3 (M6 T3) the tool number on the top right will change from T2 to T3 but the H2 still remains
is there a way that I can make it so the hight offset will always match the loaded tool?
Problem 2
When I do a tool change the z will move to the G28 position but not the xy position
I need it to move to the xyz position so it moves the job out of the way to give me space to remove the tool
I then made a m6 macro file and put in this:
M5
M9
G28
M6
This worked however every time i get an M6 it will move to this position
I think that there should be a way that it will skip the m6 if it has the correct tool in it all ready and run it if it hasn't got the right tool it in (then set the height off set at the same time)
is this possible?
For your information
I am using enroute to make my G code,
it is outputting a tool change like this:
N10 M25 G49 G17 G40
N20 T1 M6
N30 S2500 M3
N40 G0 X45. Y10. Z3.
N50 G1 Z-0.1 F200
N60 X80.
N70 Y80.
N80 X10.
N90 Y10.
N100 X45.
N110 G0 Z3.
N120 T2 M6
N130 S2500 M3
N140 G0 X45. Z3.
N150 G1 Z-0.1
N160 X90.
N170 Y90.
N180 X0.
N190 Y0.
N200 X45.
N210 G0 Z3.
N220 G40
N230 M5
N240 M9
N250 G80
N260 M30
- Attachments
-
- report_0035FF8A54EF-0717203544_2020-10-24_14-55-31.zip
- (598.97 KiB) Downloaded 142 times
-
- Posts: 728
- Joined: Mon Feb 19, 2018 2:52 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 38D269594F9C-0110180512
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: UK
- Contact:
Re: Acorn Tool Height offset problem
When you change tool, you use G43 H3 or G43 T3H3. The "H" is critical, otherwise the tool length offset (TLO) isn't set. It doesn't matter for TLO if you change tool number Tx, what matters is the TLO number Hx.
It's the G43 you need, above all. Look up the G and M codes in the CNC12 manual and see how they are used.
It's the G43 you need, above all. Look up the G and M codes in the CNC12 manual and see how they are used.
Re: Acorn Tool Height offset problem
It is an unusual (and in my opinion, deficient) post that does not include a G43 H_ code after each tool change.
Yes, you could work around this by putting a G43 code in a custom M6 macro, but you shouldn't have to.
Yes, you could work around this by putting a G43 code in a custom M6 macro, but you shouldn't have to.
-
- Posts: 17
- Joined: Mon Aug 24, 2020 6:18 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
Re: Acorn Tool Height offset problem
this is so odd to me as every cnc machine I have used the high off set when the tool is set.
is there any reason that you would every want to not change the tool offset between tools?
Seams like this should be an option in there to make it do what I want.
is there any way I can make it skip the tool change if it has the correct tool in all ready?
is there any reason that you would every want to not change the tool offset between tools?
Seams like this should be an option in there to make it do what I want.
is there any way I can make it skip the tool change if it has the correct tool in all ready?
-
- Posts: 17
- Joined: Mon Aug 24, 2020 6:18 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
Re: Acorn Tool Height offset problem
this is so odd to me as every cnc machine I have used the high off set when the tool is set.
is there any reason that you would every want to not change the tool offset between tools?
Seams like this should be an option in there to make it do what I want.
is there any way I can make it skip the tool change if it has the correct tool in all ready?
is there any reason that you would every want to not change the tool offset between tools?
Seams like this should be an option in there to make it do what I want.
is there any way I can make it skip the tool change if it has the correct tool in all ready?
-
- Posts: 17
- Joined: Mon Aug 24, 2020 6:18 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
Re: Acorn Tool Height offset problem
ok So I have been playing around to night and finally understand now how this works using the reference tool
I think that where i was going wrong was when changing tool I was not selecting the hight offset
my problem now is that I dont have a way of changing the enroute post unless any one on here might have one that thay can share?
I have read in the manual that there is some info about if The machien has a auto tool changer and a tool is set this way the software will auto select to right tool hight with the right tool.
is this right?
is there any way I can use this setting to bodge it to work how i want?
Thanks for your help
I think that where i was going wrong was when changing tool I was not selecting the hight offset
my problem now is that I dont have a way of changing the enroute post unless any one on here might have one that thay can share?
I have read in the manual that there is some info about if The machien has a auto tool changer and a tool is set this way the software will auto select to right tool hight with the right tool.
is this right?
is there any way I can use this setting to bodge it to work how i want?
Thanks for your help
Re: Acorn Tool Height offset problem
In your M6 macro, you can add "G43 H#4120" to activate the tool height offset of the same number as the requested tool.
-
- Posts: 17
- Joined: Mon Aug 24, 2020 6:18 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
Re: Acorn Tool Height offset problem
amazing it worked
I went a bit further and changed it to this:
;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;
; File: mfunc6.mac
; Desc: Tool change macro for manual tool changer but will auto change hight offset to match tool number
;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;
; Variable Definitions:
;#150 = Tool currently in the spindle
;skip if graphing or searching or if at the same tool
IF [[#4120] == [#150]] || #4202 || #4201 THEN GOTO 500
IF (#150 == 0) THEN #150 = 1 ; Initialize tool
M25 ; Run Move to tool change height Then G28 tool change position as per m25 macro
M200 "Please remove Tool %f and insert Tool %f Then Press Cycle Start to continue" #150 #4120 ; This should be Stop for Operator, Prompt for Action where i can type a comment
G43 H#4120
IF #50001 ; Prevent lookahead from parsing past here
#150 = #4120 ; update new tool number in to current number
N500
So if the current tool is correct it skips and it moves to a position befor the change
thank you for your help
I went a bit further and changed it to this:
;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;
; File: mfunc6.mac
; Desc: Tool change macro for manual tool changer but will auto change hight offset to match tool number
;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;
; Variable Definitions:
;#150 = Tool currently in the spindle
;skip if graphing or searching or if at the same tool
IF [[#4120] == [#150]] || #4202 || #4201 THEN GOTO 500
IF (#150 == 0) THEN #150 = 1 ; Initialize tool
M25 ; Run Move to tool change height Then G28 tool change position as per m25 macro
M200 "Please remove Tool %f and insert Tool %f Then Press Cycle Start to continue" #150 #4120 ; This should be Stop for Operator, Prompt for Action where i can type a comment
G43 H#4120
IF #50001 ; Prevent lookahead from parsing past here
#150 = #4120 ; update new tool number in to current number
N500
So if the current tool is correct it skips and it moves to a position befor the change
thank you for your help
-
- Posts: 15
- Joined: Sat Dec 12, 2020 9:15 am
- Acorn CNC Controller: No
- Allin1DC CNC Controller: No
- Oak CNC controller: Yes
- CNC Control System Serial Number: Add later
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
Re: Acorn Tool Height offset problem
Hi I could use some help here. I am not experienced with gcode never done it. let the post processor do it for me and frankly no time to learn it as im now 2 months behind because of installing an oak system. now that im cutting metal Im faced with the tool height offset system. never used anything like it, I love it but the machine doesnot recognize the hight differences. I added the g43 n#4120 in various ways and got various errors. dosent recognize the command or or exceeds z axis limit so forth. I am including the post processor wording/gcode the post processor output .nc and the screen shot of error message. for now its one tool at a time because frankly I cant wait. Thanks to anyone who can help and best for me If you could put exactly what should go into the post processor tool change. thanks again. btw I love the oak control on my hurco km3 knee mill. outstanding performance.
-
- Posts: 728
- Joined: Mon Feb 19, 2018 2:52 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 38D269594F9C-0110180512
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: UK
- Contact:
Re: Acorn Tool Height offset problem
Perhaps I'm confused but I don't understand why you have an extra, solitary zero on the end of line N28. Could that be the unexpected character?
Try deleting it and seeing if the error message still happens. That might give us a clue what the problem is or whether I'm just seeing a red herring.
Try deleting it and seeing if the error message still happens. That might give us a clue what the problem is or whether I'm just seeing a red herring.