Hello all,
I have successfully install and wired my acorn CNC board and love how easy it was. I must be doing something wrong when it comes to manual tool changes from the MDI function. This is what I happens.
If I load a file that has a tool change command (T005 M6) everything is fine, it runs z to the tool change position and I change the tool. The system changes the tool number AND I see tool height offset that I setup of H005. However, if I do a tool change from the MDI with the same command (T005 M6) it recognizes the tool change but does not get the z height offset and displays "T005 --". This results in an incorrect tool offset and I have crashed a few tools trying to work it out.
As I said, I am sure I must be doing something wrong as it works great from a fusion360 generated nc file, just not from the MDI.
Any assistance would be greatly appreciated.
Thank you in advance.
MDI tool change not getting tool offset (Resolved)
Moderator: cnckeith
-
- Posts: 3072
- Joined: Tue Mar 22, 2016 10:03 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: Yes
- CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192 - DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Boston, MA
- Contact:
Re: MDI tool change not getting tool offest
Have you looked in your Fusion file at the tool chsnge command? Tool change commands are in the form of Tnnhh where NM is the tool number and by is the height offset.
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.
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.
-
- Posts: 573
- Joined: Wed Aug 29, 2018 11:15 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 985DADEB24D5-0309180716
- DC3IOB: No
- CNC11: No
- CPU10 or CPU7: No
Re: MDI tool change not getting tool offest
Loading a tool and activating the tool height offset of the tool are two different steps. If you look at your Fusion 360 job file, you will see something like this:power67 wrote: ↑Sun Sep 20, 2020 1:28 am If I load a file that has a tool change command (T005 M6) everything is fine, it runs z to the tool change position and I change the tool. The system changes the tool number AND I see tool height offset that I setup of H005. However, if I do a tool change from the MDI with the same command (T005 M6) it recognizes the tool change but does not get the z height offset and displays "T005 --".
Code: Select all
N35 T3 M6
N45 S2500 M3
N50 G54
N55 M7
N65 G0 X-26.502 Y-28.629
N70 G43 Z15. H3
You need to be careful that the H# matches your Tool# in the CNC12 Tool Library.
By default the CNC12 Tool Library matches the D# and H# to the Tool# but it is possible to mess around with these assignments. As an example, you can assign D3 and H4 to T1 (see screenshot below) which makes things really complicated.
You need to make sure that the Fusion 360 Tool Library you are using matches the same assignments and YES, you can actually assign a different D# and H# to a Tool in the Fusion 360 Tool Library as seen in the screenshot below and if you browse the Forum there are people who had problems with Tool Offsets because they added the wrong H# to their Tool in Fusion.
My recommendation is: Don't mess with the D# and H# assignments in the CNC12 Tool Library and always make sure your Fusion Tool Library matches the settings of the CNC12 Tool Library.
If you use my Fusion360 Post Processor for CNC12, you can enable the Post Processor Property that will check at the beginning of a job if the tools match the settings in the CNC12 Tool Library. Check it out here
-swissi
Last edited by swissi on Sun Sep 20, 2020 11:57 am, edited 1 time in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp
Contact me at swissi2000@gmail.com
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp
Contact me at swissi2000@gmail.com
-
- Posts: 7
- Joined: Sun Sep 20, 2020 1:14 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
Re: MDI tool change not getting tool offest
Swissi,
You hit it on the head. Thank you, I thought that the height offset was "automatic" with the m6 command. now I just use the tnnn m6 Hnnn command and away it goes as expected.
Thanks for the quick response from all.
So far, I am loving the ease of install and configurability of the acorn board. at some point I will post some pics of my setup. It would not have been this nice and easy with other systems and boards. Heck, it was even easier than some of the 3d printers I have built with custom boards.
You hit it on the head. Thank you, I thought that the height offset was "automatic" with the m6 command. now I just use the tnnn m6 Hnnn command and away it goes as expected.
Thanks for the quick response from all.
So far, I am loving the ease of install and configurability of the acorn board. at some point I will post some pics of my setup. It would not have been this nice and easy with other systems and boards. Heck, it was even easier than some of the 3d printers I have built with custom boards.
-
- Posts: 237
- Joined: Wed Apr 01, 2020 8:23 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 1702
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
Re: MDI tool change not getting tool offset (Resolved)
I had the same issue. I used to have it set up in Mach 3 so that T number and H offset matched on the same line. I also crashed a tool. Following advice is from memory I did it a long time ago.
In fusion 360 you have a set of options for the tool processor that you can change. Go to the menu and turn off "preload tool". This fixed it for me.
In fusion 360 you have a set of options for the tool processor that you can change. Go to the menu and turn off "preload tool". This fixed it for me.
-
- Posts: 573
- Joined: Wed Aug 29, 2018 11:15 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 985DADEB24D5-0309180716
- DC3IOB: No
- CNC11: No
- CPU10 or CPU7: No
Re: MDI tool change not getting tool offset (Resolved)
I can't see how this fixed your problem. What the "preload tool" option does is the following:Upnorth wrote: ↑Mon Sep 21, 2020 7:11 am I had the same issue. I used to have it set up in Mach 3 so that T number and H offset matched on the same line. I also crashed a tool. Following advice is from memory I did it a long time ago.
In fusion 360 you have a set of options for the tool processor that you can change. Go to the menu and turn off "preload tool". This fixed it for me.
Right after the M6 command, Fusion inserts a Tx command, like shown in block N40 above, to "preload" the next tool that will be needed in the job file. Now what CNC12 does with this I call it a design flaw but Centroid might disagree with this statement .N35 T3 M6
N40 T1
N45 S2500 M3
N50 G54
N55 M7
N65 G0 X-26.502 Y-28.629
N70 G43 Z15. H3
If you look on top of the CNC12 screen, you will notice that the N40 block will change the T3 that was just loaded to T1 but the active tool in the spindle is still T3 and the job file will correctly activate the height offset H3 in block N70 but CNC12 will display T1 H3 on top.
The job will run correctly with T3 H3 as long as you don't have any scripts that look for the active tool in the spindle.
If you look at the CNC12 documentation, there's a parameter #4203 "Tool in Spindle" that does not exist in a regular Acorn CNC12 install and will return an error message if you try to access it and parameter #4120 that everybody uses in their scripts will return T1 and not T3 so if you are running a script that's uses #4120 you might not getting the information you expected.
There's currently just no way that I know of that CNC12 can tell you what tool is actually in the spindle. If you are using "tool preloading", you have to track it yourself in a variable.
So my recommendation for now, if you are running a regular CNC12 without a tool changer, make sure your Post Processor doesn't add any "Tool preloads" to your job file.
-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp
Contact me at swissi2000@gmail.com
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp
Contact me at swissi2000@gmail.com
-
- Posts: 237
- Joined: Wed Apr 01, 2020 8:23 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 1702
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
Re: MDI tool change not getting tool offset (Resolved)
Like I said it was a long time ago so I may not be remembering exactly correct. Tool preload was automatically applied I did not select it. I turned it off in fusion. It is also possible the program ran incorrectly for some reason. I have not had the issue repeat for a long time now.