Tool Length offsets and Part offsets

All things related to Centroid Oak, Allin1DC, MPU11 and Legacy products

Moderator: cnckeith

Post Reply
CrossfireX
Posts: 23
Joined: Sun Feb 18, 2018 7:47 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900998
Location: Mackay, Australia

Tool Length offsets and Part offsets

Post by CrossfireX »

HI guys, I've just (almost) completed a retrofit from Anilam to Centroid Oak on a large bed mill, and it's been running very well in the early stages, but I keep having a reoccurring issue that I'm hoping someone with a bit more centroid experience can help me with.

I followed CNCSNW's tool length offset procedure(s) http://www.cncsnw.com/OLEM.htm and I have sort of stuck with Method 2. but I have an issue where, sometimes, it won't get the offset right no matter what. for example: I crashed a drill this morning first thing after carefully setting the length offset and the part offset had been set (I always set offset #2 as the back left top corner of my vise hard jaws) and I checked the offset after setting my tool length offset off the machine bed as normal, but then during drilling the machine just ran full rapid into the surface of the part. I checked my ossefts and everything was fine, the numbers were negative where they were supposed to be, I couldn't find anything wrong. so I used tool #1 (my dial) and re-dialed in the part, it was spot on, just for checks and balances I checked the length of tool #1, all good. Then I changed drill bit and reset the offset as per normal, then re-did the part offset as per the procedure, but even after re-zeroing the part with the tool in the machine as per CNCSNW's method, now the tool at X0Y0Z0 is 300mm off the top of the part. I'm starting to lose my mind. I had this same problem last week with a tool, and I removed and re-set every tool in the carousel, then everything was fine, I don't want to have to do that every time I add a new tool.

does anyone know what I'm doing wrong and what is the best way to sort my tool offsets? I don't have a touch probe or anything, I just use a piece of shim stock on the machine bed, I keep the same 10 or so tools in the carousel all the time, the only time I change anything is if I have to replace a worn endmill of I'm using a small twist drill in my drill chuck.
If the green light ain't burning, you ain't earning.

Jason A.K.A. CrossfireX
CrossfireX
Posts: 23
Joined: Sun Feb 18, 2018 7:47 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900998
Location: Mackay, Australia

Re: Tool Length offsets and Part offsets

Post by CrossfireX »

Hi Everyone reading this, I may have solved my own problem, but I'll pass it on to anyone else having the same or similar issues.

when doing a manual tool change (using the ATC button, or using the MDI console) the tool changes but the offset doesn't, for example: If I have tool #10 in the spindle and I change to tool #19, it will physically change to tool #19 and in the top of the screen it will say tool #19 but will keep the offset of tool #10 (H10). it doesn't do this during a program, only when doing it manually through the console. I'm not sure why this is happening, and i'll look further into it, but at least now I know I need to manually set the offset every time I do a manual tool change.
If the green light ain't burning, you ain't earning.

Jason A.K.A. CrossfireX
cncsnw
Posts: 2080
Joined: Wed Mar 24, 2010 5:48 pm

Re: Tool Length offsets and Part offsets

Post by cncsnw »

In G code, tool numbers (T codes) and height offsets (H codes plus the G43/G49 state) are entirely separate things.

It is, therefore, expected that "M6 Tnn", whether in a CNC program or at the MDI prompt, will only change tools, and will not change height offsets.

Optionally, you can set CNC12 to automatically activate the corresponding height offset when you use the F7/ATC key. To do so, set Machine Parameter 3 to a value of 4. This will also have the effect of leaving any active height offset active when you visit the Offset Library screen. By default, height offsets are always cancelled when you enter the Offset Library.
CrossfireX
Posts: 23
Joined: Sun Feb 18, 2018 7:47 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900998
Location: Mackay, Australia

Re: Tool Length offsets and Part offsets

Post by CrossfireX »

Thanks Marc, I've never had to do that before, I guess normally you call a tool and it has a default offset, and then if you want a different offset for that tool you call it, like if you're doing progressive gun drilling, you use the same tool just call different offsets every time you change your drill. Now that I know what the problem is I've been able to work around it by just going into the tool offset library and back out and it clears the offset. since I figured out that little trick I've had no problems. It's just something you I to get used to I guess.

As mentioned, when running a job, there are no problems, only when using the ATC function or the "m6 t#" command in MDI. It cost me a drill bit and a small job, but it's a cheap price to pay for learning what the problem is. Now I know I'll keep a more careful eye on the offset.
If the green light ain't burning, you ain't earning.

Jason A.K.A. CrossfireX
Post Reply