qtdragon - probing issues

hey, one more thing with the probing routines.....
all the dimensions and distances, etc., should be displayed as 4 decimal places. like 1.2345
and used internally even better, maybe at least 6 places.....
all the round offs can really add up
i'm trying to cut bearing bores, with +-.0002 accuracies...

and another small question.... can the NCGUI_SUBFILE_PATH have more than one entry? like the regular SUBROUTINE_PATH ??? with : separators?

gotta keep at this.     it took a bunch of years for axis to get worked out.....

Roguish wrote:

gotta keep at this.     it took a bunch of years for axis to get worked out.....
​​​
 

Agreed. This is an amazing interface already. 
There is a lot of refinement I can see could be done in the probing routines but let's get it working first!

Re accuracy:
What is the repeatibility of your probe? 
What is the resolution of your machine?
Three digits is nice for metric machines. That's down to 1 micron, same as a Reinshaw.
Some of us are using probes with  resolution much worse than that.

I am no expert but I'm pretty sure you could change the number format yourself just by altering the stylesheet. Hit F12 and you will see what I mean...
 

Roguish wrote:

hey, one more thing with the probing routines.....
all the dimensions and distances, etc., should be displayed as 4 decimal places. like 1.2345
and used internally even better, maybe at least 6 places.....
all the round offs can really add up
i'm trying to cut bearing bores, with +-.0002 accuracies...

and another small question.... can the NCGUI_SUBFILE_PATH have more than one entry? like the regular SUBROUTINE_PATH ??? with : separators?

gotta keep at this.     it took a bunch of years for axis to get worked out.....
 

Ok pushed numerical format changes - inch based machines have 4 digits, metric 3 (in feature branch)

Only one NCGUI_SUBFILE_PATH can be specified.
 

Rodw,
I definitely get and agree with your points.  I try to be as realistic and pragmatic as possible.
The little cheap chinese benchttop mill I'm working on now certainly has it's limits, and I've found them painfully.
For the last several weeks I have been fighting spindle runout.  I measured it when the mill was new and it was about 0.0008 inches.  not too good, even for a cheap benchtop.  So I decided to change out the bearings....after doing that and reassembling the spindle and quill assembly, the runout shot up to 0.0025 inches.  Horrible.  After disassembling and reassembling a few times, with no improvement, I contacted the distributor.  After a number of back and forth communications, including photos and videos of the measurements, the distributor kindly sent me a new spindle shaft from the manufacturer.  The spindle has 2 angular contact bearings with spacers on the shaft, and that is inside the quill with an end cap.  The parts drawing from the manuf is not detailed enough to tell exactly how the bearings should be configured.  face-to-face, or back-to-back, with the spacers in between.  After a lot of head scratching and searching and reading I found some really good docs from Nachi (a Japanese bearing manuf).
I carefully measured everything as good as I could, and reassembled with a couple of shims between the bearings, and under the quill end cap to press on the bearing's outer races.  After several shim adjustments, I got the runout down to 0.0004 inches.  phenomenal for this type and quality of mill.  I'd really like the runout to be much small, but that's just not reasonable....and that is with the original spindle shaft.  I will probably return the replacement shaft.
I have also been struggling with my probes (I have 2) to get them centered.  Again, I'd like them to be perfect, but that's also not reasonable.  My target is about +-.0002,  I'm getting close, but it takes an inordinate amount of effort.  I'm also looking at compensation methods and I think I have found one that is reasonable and doable.
All in all, I am working hard at being reasonable with my expectations.  Which is something I tell noobies frequently on the IRC channels.
I also have a Series II Bridgeport.  5500 pounds of steel, and stiff as a hell.  Whatever I do on the small mill will probably migrate to the big mill.

Managing expectations and requirements is key to success.  I've been a professional engineer for 40+ years and worked on a huge variety of projects, so I really do get it.
I do appreciate your assistance and advice, and your common sense and pragmatism.  Both rare qualities these days......
 

Roguish wrote:

Rodw,
I definitely get and agree with your points.  I try to be as realistic and pragmatic as possible.
The little cheap chinese benchttop mill I'm working on now certainly has it's limits, and I've found them painfully.

Managing expectations and requirements is key to success.  I've been a professional engineer for 40+ years and worked on a huge variety of projects, so I really do get it.
I do appreciate your assistance and advice, and your common sense and pragmatism.  Both rare qualities these days......

 

Great work on the spindle bearings. Did you measure runout on the spindle inside taper? Once I fitted a collet chuck to a Chinese lathe which is the only time runnount became important for me. I found the inside taper had absolutely zero runout. So any runout I experienced was of my own doing. I eventually got it but even tightening the chuck mounting bolts affected runout. The manufacturer of my cheap Chinese probe was at pains to point out the collet used could introduce runout.

Oh, yeah, measured all over. but in the taper was most important.
everything has runout, it's all a matter of how much.....

Ok, Back on topic!

Chris,
I've been through all of the basic probe routines except inside corners and edge angle.
there is  a regression on the height probe as its adding the extre depth in again
All other probing worked OK

I have yet to master small hole probing but at 40mm diameter its fine.

I have not looked at versby. I'm hoping Rougish has that side covered. It might be a few days before I can get back to testing.
I have a panel mount monitor that just arrived which takes precadence.

Suggestion: We have a field on the probe page for our probing tool number. 
It would be nice to have a M61 Qn button on the probe screen so we can load that tool.

I don't see regression on the code here. Were you on the right branch?
probe_down should finish at Z clearance.

Looking at hole probe in basic the first few moves::
- move down Z clearance + extra depth
- move over 1/2 diameter hint - xy clearance.
- negative probe at max xy probe length (finish at latch return distance away from edge)
- move 2 x (1/2 diameter - xy clearence) <<< this seems wrong
- positive probe at max xy probe length

m61 button would be good on a non ATC machine but a disaster otherwise.
There is a M61 button on the tool page

I assumed I would be still on the same branch after a git pull but I'll check tomorrow.


I would like to eliminate any G1 moves in a hole unless returning to a known safe position. My probe has a maximum recommended velocity of 200mm so I don't want to exceed that.

Something like:
- move down Z clearance + extra depth
- negative G38.2 X axis probe diameter hint x 1.5
- probe away slow G38.4 X(distance to start), record pos
- positive G38.2 probe X axis probe diameter hint x 1.5
- probe away slow G38.4 X(distance to start), record pos
- return to calculated X centre
- negative G38.2 Y axis probe diameter hint x 1.5
- probe away slow G38.4 Y(distance to start), record pos
- positive probe Y axis probe diameter hint x 1.5
- probe away slow G38.4 Y(distance to start), record pos
- return to calculated X,Y centre
- raise to clearance height (could combine with previous move if brave)

This will be much more efficient and using G38.4 should give more accurate results and simplify the code. Just record the position and head for the other side.. What do you think?

Re M61 Qn: qtdragon should know (or could be told via the ini file) if a manual toolchanger is in use. Perhaps it could unhide a button in this case?

I don't want to completely change the probe routines - it's complicated code that I don't know well. And i never know when linuxcnc decides it will be released
More efficient ones will have to wait for master.

It seems to me, what you are saying - small hole probe should skip the rapid positioning.
Don't want to get rid of rapid completely in case you are probing large holes.
Two ways I can think of that are pretty easy:

1) have probe calculate based on diameter hint and probe diameter when to skip the rapid positioning move. say if diameter is < 4x probe diameter - skip rapid

2) have the user set xy clearance to zero or (diameter to zero?) would cause skipping of rapid positioning

I think in the future the data entries should remember settings based on the displaed probe buttons. meaning if you switch between hole probing and edge probing then clearance etc could be different without having to physically change them each time.

yes I suppose a button that either does M61 or m6 based on a preference setting.