Struggling with lathe tool auto touch off with tt not at centerline

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Muzzer
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:

Struggling with lathe tool auto touch off with tt not at centerline

Post by Muzzer »

I thought I was doing quite well coming to terms with the auto touch off procedure in CNC12 lathe but today when I come to the machine I find myself completely at a loss.

I managed to touch off the first 4 tools in my turret last weekend and sure enough, when I requested a tool change to those tools, the correct offsets were applied. So today I was hoping to move on from std external turning tools to boring bars and drills in positions 5-8 but when rerunning the touchoff process as a sort of refresher on an external tool, today I find the X offsets being reported are way out.

Most of the tools are 125mm length, within 1mm or so and the X offsets were all coming in at around the -70mm mark. But when I try to repeat those same offset measurements in a spare tool table position today while using tool #1, the reported / measured offset is -140mm. That is suspiciously double the previous value.
20221202_190919.jpg
20221202_190939.jpg
I've tried to figure out what I'm doing wrong or what is changed. When I call a new tool / index the turret, the previous offsets make sense when applied but sure enough, the new tool with the -140mm offset has the diameter coordinate out by 70mm.

One (other!) area of confusion is the use of absolute vs relative measurements during tool touchoff. I was hoping this might be the root of the issue but unfortunately it doesn't seem to matter which one I choose.

Being familiar with CNC12 mill, I was expecting a similar "reference tool" concept and planned to use tool #1 as a reference tool but that doesn't seem to be how it's done here.

It doesn't seem likely to be helpful to post my current report although I could do if you think otherwise. I think this is a question of RTFM on my part but despite doing so and watching the vids by Keith and Uwe, I'm not wiser. I'm hoping it's fairly obvious to a seasoned user where I'm going wrong. The manual section on auto touchoff is very brief.
slodat
Posts: 793
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Struggling with lathe tool auto touch off

Post by slodat »

Following along. I bought the TT-4 for lathe and could not figure out the auto tool measure routines. I’m measuring manually and it’s working perfectly.
suntravel
Posts: 1967
Joined: Thu Sep 23, 2021 3:49 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 6433DB0446C1-08115074
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Germany

Re: Struggling with lathe tool auto touch off

Post by suntravel »

What version of CNC12 you are running?

4.62 had a bug in Auto Tool Touch off Lathe, so pls. install the current 4.82

Workflow for Auto Measure

Skimcut, set Part Reference X

Set Ref X and Z with the same tool in the tool lib

Auto measure all tools except Drills and Taps, they only in Z

To measure Drill and Taps in X use a dial indicator or Centricator in the spindle to finde X0

Ref X manual to X0 and manual measure X

Make parts :)

Uwe
Muzzer
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: Struggling with lathe tool auto touch off

Post by Muzzer »

That's interesting, Uwe. I'm running 4.80 - I wonder when the bug was fixed. I'll update to 4.82 and see if that improves matters.

I'm planning to mount my probe as shown in the tailstock, as the hydraulic chuck isn't easy to mount a probe on. Equally, skimming a part and measuring it isn't how I'd like to do this if I can avoid it. The thumbnails show a reference tool being used for both X and Z offsets, so I can't imagine why I can't use offsets relative to a reference tool (perhaps tool #1).

I also found I had to select nose vector 6 for the boring bar to get the correct X direction move (it is shown crossed out). Interestingly, that resulted in a more sensible looking offset (~56mm as opposed to -140mm, despite the tips being nowhere near 42mm physically distance apart).
suntravel
Posts: 1967
Joined: Thu Sep 23, 2021 3:49 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 6433DB0446C1-08115074
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Germany

Re: Struggling with lathe tool auto touch off

Post by suntravel »

With precise homing, you must set part X Ref only once.

I prefer Skim Cut, but you can also do this with the probe, cut test part, measure and loop till it fits ;)

Uwe
Muzzer
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: Struggling with lathe tool auto touch off

Post by Muzzer »

I think I'm getting there now. I was planning to update from 4.80 to 4.82 but TBH I can't see any suggestion from the release notes that anything has been done that would affect lathe touch off. Besides, I now have a custom PLC on account of my ATC turret, which would further complicate matters.

Instead, I've done some experimentation / learning / calculations to better understand what is going on and I seem to have made some progress.

I started out by setting Xref to zero at the point of touch off of Tool #1, which I'm considering to be my reference tool. I'm not sure why I'd do this from what I've read in the manual but it seemed sort of in line with what Uwe said just now. Subsequently, the offsets are back around the -70mm for the external tools. But I still couldn't understand the boring bar offset.

On my machine, the boring bar tip is ~26.5mm closer to the turret axis (ie in radius units) than the external tools. That's equivalent to a difference of ~53mm in diameter. My probing "tip" is actually a piece of 3/8" square stock (so that I can probe it from all sides unlike a ball tip) ie 9.53mm across flats. The section in the CNC12 lathe manual dealing with boring bar offset measurements says "multiply the [boring bar] manufacturer’s offset by negative two (-2), and type the number into the X Offset field. The value you type should appear as being added to the measured X offset already measured." This seemed to be pretty relevant and indeed my "offset problem" distance is twice the width of the probe tip.

Quite simply, if I subtract twice the width of the probe "tip"(ie a total of 19.06mm) from the offset, I end up with the "correct" offset. By way of a check, when I change tools and approach a fixed DTI, the typical final "error" in the DRO position between my external tools and the the boring bar is 19mm before this correction is implemented.

So (and yes, I'm still new to CNC12 lathe):
  • Offsets are measured as diameter units, not radius.
  • As suggested by Uwe, the Xref should be entered only once. I can't say I'm quite clear how this works yet but it's a start.
  • The auto touchoff process doesn't seem to allow for the width of the probe tip when measuring boring bar / internal tools.
  • That's likely because the process outlined in the CNC12 lathe manual tells us to manually enter the boring bar offset. This is essentially the same process used for drills and taps but with the offset entered manually.
  • The manual covering lathe tool auto touch off is "commendably brief".
  • When I auto touch off boring bar tools with my probe, I will need to subtract twice the width of my probe.
Phew. Probably quite a simple problem but it took me some head scratching to figure out!
cnckeith
Posts: 7166
Joined: Wed Mar 03, 2010 4:23 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: none
DC3IOB: Yes
CNC11: Yes
CPU10 or CPU7: Yes
Contact:

Re: Struggling with lathe tool auto touch off

Post by cnckeith »

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
Gear we use but don't sell. https://www.centroidcnc.com/centroid_di ... _gear.html
Muzzer
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: Struggling with lathe tool auto touch off

Post by Muzzer »

Yes I saw that video but although the tool library shows some boring bars, you stopped after doing an (easy) external turning tool!

Am I right in thinking that auto touch off doesn't actually work with boring / internal tools without the workaround I mentioned?

Note that on my machine, I can't simply bring the boring tool to the other side of the spindle axis, so I need to touch off on a different face (side) of the probe.
suntravel
Posts: 1967
Joined: Thu Sep 23, 2021 3:49 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 6433DB0446C1-08115074
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Germany

Re: Struggling with lathe tool auto touch off

Post by suntravel »

With a boring bar you must use the opposite side of the probe compared to turning tools.

Probing cycle and Wizard setup is also made for a probe in the centerline of the spindle.

I am not sure if it calculates with probe diameter right if off center mounted.

Uwe
Muzzer
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: Struggling with lathe tool auto touch off

Post by Muzzer »

suntravel wrote: Sat Dec 03, 2022 5:20 pm With a boring bar you must use the opposite side of the probe compared to turning tools.
That's what I've been doing. But it seems that when you do this, you need to subtract 2x the radial width of the probe because it thinks the tool tip is in the same place as it was for external tools. It would be nice if the auto probing feature did this for you, rather than requiring a manual correction.

Have you been auto touching off boring bars on your machine? Do you get sensible results?
Post Reply