Few questions on a tool setup procedure (lathe) -- does this make sense?

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

Moderator: cnckeith

Post Reply
Surgo
Posts: 9
Joined: Tue Feb 25, 2020 11:45 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
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: none

Few questions on a tool setup procedure (lathe) -- does this make sense?

Post by Surgo »

I have a lathe running CNC12 on Allin1DC. It doesn't have a turret or gang setup; instead, it has a Dorian QCTP. I also don't have the Centroid tool touch-off (though I wish I did). Instead I'm trying to hack together a rough equivalent method for automatic tool measuring using a "reference tool" (not unlike one for a knee mill), which is one of those common electronic probes that lights up and beeps when the electrical circuit is closed. I have this sitting in a dedicated toolholder. I have a second probe which is held in the chuck; it also lights up and beeps when its electrical circuit is closed, but it resembles a tool touch-off instead (has a pancake-shaped surface that can be touched on both the X and Z positions for locating).

The idea: hold probe #2 in the chuck when I want to set up tools. Put probe #1 in the toolpost. Dedicate G59 as a "scratch" coordinate system (every other one uses X = 0 as the centerline of the spindle, this one will not and instead use it as where the reference tool touches in X). Then when I want to add new tools, I perform the following operations:
  1. G59
  2. Jog the X and Z locations of the tool touch-off using the reference tool. Set these as G59's zeroes.
  3. Insert tool I want to touch.
  4. Jog its Z on the tool touch-off. Set it as the tool's Z offset in tool library.
  5. Jog its X on the tool touch-off. Set it as the tool's X offset in tool library.
  6. Repeat steps 3-5 for every tool to be measured.
  7. Insert reference tool.
  8. Insert workpiece.
  9. Jog workpiece's Z using reference tool. Set it as G59 Z-zero and G54 Z-zero.
  10. Jog workpiece's outer diameter X using reference tool. Set it as G59 X-zero.
  11. Switch to G54.
My understanding is that all of the following will be then true:
  • Any tool's cutting edge (provided radius etc are set correctly) will, when X=0, be at the centerline of the spindle.
  • Any tool's cutting edge (provided radius etc are set correctly) will, when Z=0, be at the Z end of the part.
  • The Z=0 will be the Z-end of the part.
To sum up, the idea is to use a probe set in tool #1 as a reference, first to probe the position of a setter that will record its offsets (in G59) and all the other tool offsets, and then to probe the positions of the workpiece (in G59), then with the WCS switched back to G54 all these tool offsets will still be valid. Should this work as I expect, or are there wrinkles here that I'm not seeing?

Secondly, assuming all this does work as I expect, I wrote a macro to automate the process:

Code: Select all

; Tool and part setup macro.
; Uses G59 as the scratch coordinate system to set the part X/Z (NOT CENTERLINE).

#100 = 0.125/2       ; Radius of the probe.
#101 = 1             ; Reference tool number.
#102 = -1            ; Current tool number we're probing.

N100
G59
T #101 00
M225 0 "Jog reference tool to Z location of the tool setter"
#2600 = 0
G10 P#101 Z0
M225 0 "Jog reference tool to X location of the tool setter"
#2500 = [-#100]
G10 P#101 X-#100

N200
M224 #102 "Enter tool number to probe, -1 to cancel."
IF #102 = -1 THEN GOTO 300
T #102 00
M225 0 "Jog tool to Z location of the tool setter."
G10 P#102 Z0
M225 0 "Jog tool to X location of the tool setter."
G10 P#102 X0
GOTO 200

N300
M225 0 "Press CYCLE START to probe part, cancel to exit."
T #101 00
M225 0 "Jog reference tool to Z location of the part."
#2600 = 0
M225 0 "Jog reference tool to X location of the part."
#2500 = [-#100]

N400
M225 0 "Probing and setup complete."
G54
I'm confused on one point -- lathes don't have G91/G92 for incremental/absolute mode. How can I specify, when setting the WCS parameters, that I do mean the current positions?

I'm also wondering, if there's a way to display on the screen all the existing tools at the start of the N300 block, to make life easier for the operator so they don't have to recall from memory what all the tools and their numbers are.
Last edited by Surgo on Sun Sep 19, 2021 10:30 pm, edited 1 time in total.
tblough
Posts: 1706
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: Few questions on a tool setup procedure (lathe) -- does this make sense?

Post by tblough »

Lathes use U and W for incremental in X and Z respectively.
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.
Surgo
Posts: 9
Joined: Tue Feb 25, 2020 11:45 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
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: none

Re: Few questions on a tool setup procedure (lathe) -- does this make sense?

Post by Surgo »

tblough wrote: Sun Sep 19, 2021 10:07 pm Lathes use U and W for incremental in X and Z respectively.
Thank you! That's obviously very good to know.

Not quite clear how I can use it for the parameters. For setting a tool offset, for example, can I:

Code: Select all

G10 P12 W0
instead of:

Code: Select all

G10 P12 Z0
I guess for the WCS, when I set the axis values, the immediate or calculated value I insert becomes the exact value for that axis in the WCS, regardless.
cnc_smith
Posts: 216
Joined: Mon Nov 20, 2017 10:13 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: Yes
CNC Control System Serial Number: none
Location: Frenchville, PA

Re: Few questions on a tool setup procedure (lathe) -- does this make sense?

Post by cnc_smith »

Surgo,

Your way may work but I think you are making it a little more complicated then what needs too be.

With the lathe X0.0 should always be the center of the spindle for every WCS. Not doing this could burn you and cause a crash.

Looking at your macro you have #100 = 0.125/2 ; Radius of the probe.


I am assuming the probe is your probe #1. Are you setting the center of it to X0.0? For the lathe the edge of the tool is used not the center of the radius.

Instead of setting X0.0 in G59 on the edge of the probe #2 I would do the following.

1) Measure the diameter of the disk on your Probe #2. Say it is ¾” (19mm) diameter. I would put an indicator on the edge and rotate the spindle to see how true it is running. If it is with in a couple thousand ( 100 MM) that should be close enough to work with. If you have any adjustment you can true it in. If probe #2 is running out very much this will effect you diameters when setting tools if you do not put it back in the exact orientation.

2) Using your Probe #1 as reference tool jog it over to the Probe #2 to where it is touching the OD and lights up. Now press the F1 X Diam key. This will give you the X diameter that you will be touching the OD tools off of. As noted early about measuring the probe #2 diameter this X Diam should be slightly smaller than the measured diameter depending on how much mechanical movement there is to trip it. If Probe # 2 is running fairly true you will not have to set this again for doing OD and ID tools.

3) Use this X Diam as a variable in your macro. You will take the X Diam and subtract it from the current position and assign it using the G10 as X value for the offset.



I have taken your macro and written a macro that is based on what I think you wanting to do. I have just run it on bench test. Did not have time yet to test the macro a machine. Wanted to get this out so you could look at it over the weekend. I am will be leaving shorty and will not be back until Monday.

This is one way of doing it. It can have features added such that it would prompt you if you want to do any additional tools while the Probe #2 is in the spindle. Someone may have written something similar to this and it can improved. This gives you the basics how the macro would be written.
Attachments
Measruing Tool offset using manual touchoff.txt
(2.55 KiB) Downloaded 21 times
Dana

When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
Surgo
Posts: 9
Joined: Tue Feb 25, 2020 11:45 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
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: none

Re: Few questions on a tool setup procedure (lathe) -- does this make sense?

Post by Surgo »

Thanks Dana! Using the existing diameter of Probe #2 as a variable makes a lot of sense. Why on earth didn't I think of that the first time?
Post Reply