Tool setting on my Mill

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
john543
Posts: 48
Joined: Wed Oct 06, 2021 3:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: E06234795241-0928215226
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Maine

Tool setting on my Mill

Post by john543 »

Hi all
This is gonna be short I just typed like 6 paragraphs, and someone showed up so I walked away for some time when I returned, I continued with my post and went to preview, and it erased everything I just typed. :evil:
Any way I have a Birmingham Mill that's been CNC'ed by someone else they used steppers and I changed to Clearpath, I built my controller just like Marty's Syl project just use a different VFD used clearpath motors also.

So here my problem I found the builder of the original machine said there was 5" of z axis travel and there is actually 4" of travel (crash) tore it apart fixed my crash and then realized I needed to fix my reference tool by one inch that's done measured all the tools, Done.
now I set up on a new part and used my Drewtronics S5000 to set 3 axis on the part then using the same S5000 set the top of the part. Just before I ran this program I did a g0z0 off the part to see if everything was set right well it wasn't tool moved .4732 below part zero and I've been going in circles chasing this error and now I'm here where there's smarter people than me HELP! lol.

Photo of mill
https://photos.app.goo.gl/TDd6Uhr1urc3mbLBA

John
Attachments
report_E06234795241-0928215226_2022-10-31_07-06-23.zip
(4.5 MiB) Downloaded 4 times
cncsnw
Posts: 3763
Joined: Wed Mar 24, 2010 5:48 pm

Re: Tool setting on my Mill

Post by cncsnw »

What are you using as a Reference Tool, to set Z Reference in the Offset Library?

Did you set the Z axis Part Zero (under F1/Setup -> F1/Part) before, or after, you measured the tool lengths in the Offset Library (F1/Setup -> F2/Tool -> F1/Offset Library)?

When you did "g0 z0", what tool was in the spindle? What H offset was displayed in the status window at the upper right?
john543
Posts: 48
Joined: Wed Oct 06, 2021 3:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: E06234795241-0928215226
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Maine

Re: Tool setting on my Mill

Post by john543 »

So the reference tool is a brass rod that I took my shortest tool measurement and added the Z axis travel to it 6.43".
My automatic tool setter was giving me troubles so I used a 123 block to set all my tool length's.
Then I put in the probe and probed the peice I had in the vice 3 axis after I went to part using the probe again set the part Z zero.
Now that you mentioned it the screen said T12 but no H12 I wonder why but shrugged it off.
Screen showed T12H___

Also looking at my report I know it says 10/31 date that pc is not connected to the Internet.
john543
Posts: 48
Joined: Wed Oct 06, 2021 3:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: E06234795241-0928215226
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Maine

Re: Tool setting on my Mill

Post by john543 »

I think We're good, I'm thinking it was the way I was calling the tool. If I give it a T12 M6 cycle start it wouldn't add the H12 it was set to T12 H99 .
H99 is my probe I don't doo a lot of manual tool changing so I didn't know tool change consist of T12 H12. Machines I'm use to I never had to put anything else than T12 M6
Thanks for jogging my mind

John
tblough
Posts: 3071
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: Tool setting on my Mill

Post by tblough »

You need a G43 or G44 followed by Hnn where nn is the height offset you want to us. There are two reasons why this is not automatic. First is it a positive offset (G43) or a negative offset (G44)? Second, height offset numbers do not have to be the same as the tool number. I can have T1H1, or T1H2, or T1H27.

By not tieing the tool and offset together, with the same g-code, I can mill a pocket to depth in multiple passes by just entering a different height offset number.
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.
cncsnw
Posts: 3763
Joined: Wed Mar 24, 2010 5:48 pm

Re: Tool setting on my Mill

Post by cncsnw »

If you are using normal tool-setting procedures, you always use G43, never G44.

G44 is only used in a setup where longer tools have more-negative offsets, and shorter tools have more-positive offsets.

It is not a question of whether your particular offset values happen to be positive or negative; it is a question of in which direction you are measuring and applying the offsets.
john543
Posts: 48
Joined: Wed Oct 06, 2021 3:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: E06234795241-0928215226
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Maine

Re: Tool setting on my Mill

Post by john543 »

G43 is called in my program, this was a manual tool change no program loaded at the time. Like I said after I zeroed my part I then in MDI called T12 for the tool then did a G0Z0 just checking myself on tool measurement.
Tool moved too far into the piece of stock good thing I was off to the side of the stock.
After posting here CNCSNW jogged my mind about the Hxx value. Looking back I remember seeing on the screen T12 H99 but it just didn't register in my brain. So I returned to the machine and did some tool calls in MDI and soon realized I needed to call a tool with T12 H12 if I didn't the H value would be set to the last tool called.

Like I said in my last post things are good and thank you for jogging my mind, sometimes you just need a kick in the head to fix things lol.

John
Post Reply