Re: [Emc-users] Probing

[Robin Szemeti via Emc-users]

https://www.youtube.com/watch?v=WnQV8E8Ja5E

On Mon, 28 Mar 2022 at 12:23, andy pugh  wrote:

> On Mon, 28 Mar 2022 at 03:29, Thaddeus Waldner  wrote:
>
> > Ah! I just saw that P0 is for the active coordinate system. Is P
> optional?
>
> I think that 0 is assumed if P is omitted
>
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is
> designed for the especial use of mechanical geniuses, daredevils and
> lunatics."
> — George Fitch, Atlanta Constitution Newspaper, 1912
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[andy pugh]

On Mon, 28 Mar 2022 at 03:29, Thaddeus Waldner  wrote:

> Ah! I just saw that P0 is for the active coordinate system. Is P optional?

I think that 0 is assumed if P is omitted

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Thaddeus Waldner]

I am not at the machine right now but if memory serves me right, I used
G10 L20 P1 Z1.588

Ah! I just saw that P0 is for the active coordinate system. Is P optional?


Thaddeus Waldner

From: Andy Pugh 
Sent: Sunday, March 27, 2022 7:55:07 PM
To: Enhanced Machine Controller (EMC) 
Subject: Re: [Emc-users] Probing



> On 28 Mar 2022, at 00:26, Thaddeus Waldner  wrote:
>
> I was able to get this working. Thanks for the help. I ended up using a macro 
> and modifying G54 Z offset

If you use G10 then it will use the current coordinate system.

G10 is almost always the correct in to use for this.

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Andy Pugh]

> On 28 Mar 2022, at 00:26, Thaddeus Waldner  wrote:
> 
> I was able to get this working. Thanks for the help. I ended up using a macro 
> and modifying G54 Z offset

If you use G10 then it will use the current coordinate system. 

G10 is almost always the correct in to use for this. 

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Thaddeus Waldner]

I was able to get this working. Thanks for the help. I ended up using a macro 
and modifying G54 Z offset.

My probe is actually a mechanical switch with a touch plate. I use it by 
placing it on top of the workpiece, then probing with the cutter. This machine 
has the collet attached to the spindle, so I have to set the Z offset when I 
change tools. The probe speeds up a tool change considerably.

> On Mar 26, 2022, at 7:14 AM, gene heskett  wrote:
> 
> On Saturday, 26 March 2022 02:10:50 EDT Thaddeus Waldner wrote:
>> Hi,
>> 
>> I am in the process of installing a probe on my router. I want to use
>> this by placing it on an arbitrary location on top of the workpiece
>> and probing with the installed cutter.
>> 
>> I would like to configure an unused physical keypad button to run a
>> probing routine that will probe, then automatically adjust either a
>> workpiece offset or a tool offset.
>> 
>> At this point I have the probe connected and switching the
>> motion.probe-input signal; G38.2 works.
>> 
>> Can someone show me what is required to make the rest work? I imagine
>> that I should write the probing routine in g-code and run it at the
>> push of the button … somehow.
>> 
>> Thaddeus Waldner
> 
> Andy may have a better idea, but I would explore the idea of running a 
> named subroutine that captures the machines current xy position, (so you 
> can run it up the post and return to the saved xy position) moves to the 
> contact pad, starts the spindle slowly in reverse so it doesn't cut the 
> pad, does the g38.2, and uses the results to set the coordinate system Z, 
> probably with an offset from the known height of the pad. I use un-etched 
> pcb material for the pad which is about 1/16" thick. 99% of this, var 
> #numbers etc is in the Documentation.pdf. Okular will be your friend.
> 
> Cheers, Gene Heskett.
> -- 
> "There are four boxes to be used in defense of liberty:
> soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author, 1940)
> If we desire respect for the law, we must first make the law respectable.
> - Louis D. Brandeis
> 
> 
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[gene heskett]

On Saturday, 26 March 2022 02:10:50 EDT Thaddeus Waldner wrote:
> Hi,
> 
> I am in the process of installing a probe on my router. I want to use
> this by placing it on an arbitrary location on top of the workpiece
> and probing with the installed cutter.
> 
> I would like to configure an unused physical keypad button to run a
> probing routine that will probe, then automatically adjust either a
> workpiece offset or a tool offset.
> 
> At this point I have the probe connected and switching the
> motion.probe-input signal; G38.2 works.
> 
> Can someone show me what is required to make the rest work? I imagine
> that I should write the probing routine in g-code and run it at the
> push of the button … somehow.
> 
> Thaddeus Waldner

Andy may have a better idea, but I would explore the idea of running a 
named subroutine that captures the machines current xy position, (so you 
can run it up the post and return to the saved xy position) moves to the 
contact pad, starts the spindle slowly in reverse so it doesn't cut the 
pad, does the g38.2, and uses the results to set the coordinate system Z, 
probably with an offset from the known height of the pad. I use un-etched 
pcb material for the pad which is about 1/16" thick. 99% of this, var 
#numbers etc is in the Documentation.pdf. Okular will be your friend.

Cheers, Gene Heskett.
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis





___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[andy pugh]

On Sat, 26 Mar 2022 at 06:14, Thaddeus Waldner  wrote:

>  I imagine that I should write the probing routine in g-code and run it at 
> the push of the button … somehow.

Have a look at MDI_COMMAND in the INI config.

There are a set of input pins that will trigger a line of G-code when toggled.

You need more than one line, so need to call an O-word subroutine.

Then G10 can be used to set the work or tool offset.


-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Kenneth Lerman]

Hi Gene,

I gave up on centering my cheap probe because it really isn't necessary. I
don't need the probe to be concentric with the spindle if I know the
offset. My procedure is:

   - center a hole under the spindle. For a hole, I've created a fixture
   with a magnet holding a bearing. To center it, I put the right size drill
   rod in a collet in the spindle
   - Find the center of the hole with the probe and save the coordinates.
   - Now rotate the probe 180 degrees. To do that, I've added wings to my
   probe that contact a vertical rod on the side of my mill.
   - Find the center of the whole with the probe. The difference in the two
   readings represents twice the X and Y offsets of the probe.
   - Now when you use the probe, you can just subtract that offset from the
   actual measurement.

I've written subroutines to do that and to save the offset values. I also
have probing routines to do things like finding centers, finding edges,
etc. Those routines are invoked by buttons on my pendant. Unlike Verser's
routines all probing motions are "safe". By safe, I mean that all motions
use the probing versions of motion so they stop when the probe hits
something. (I bent my first probe using Verser's routines.) The probing
routines know about the direction of the last motion directed by the
pendant, so they probe in that direction.

See: safe probe source


Ken


Kenneth Lerman
55 Main Street
Newtown, CT 06470



On Sun, Oct 24, 2021 at 1:19 PM Gene Heskett  wrote:

> On Sunday 24 October 2021 11:30:07 Feral Engineer wrote:
>
> > I use work with probe, but I am going to customize the routines a
> > little to work the way I want them to and Andrew Beck I believe uses
> > his probes.
> >
> > Phil T.
> > The Feral Engineer
> >
> > Check out my LinuxCNC tutorials, machine builds and other antics at
> > www.youtube.com/c/theferalengineer
> >
> > Help support my channel efforts and coffee addiction:
> > www.patreon.com/theferalengineer
> >
> > On Sun, Oct 24, 2021, 11:01 AM andy pugh  wrote:
> > > On Sun, 24 Oct 2021 at 08:02, John Dammeyer 
> > >
> > > wrote:
> > > > Is anyone using
> > > > https://github.com/verser-git/probe_screen_v2
> > > >
> > > > Any comments about it?
> > >
> > > About 50 pages of comments here:
> > >
> > > https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-pr
> > >obe?start=0
> > >
> > > Verser also sells relatively inexpensive touch-probes:
> > > https://vers.by/en/16-touch-probes
>
> I don't think its a verser product, but the plastic one I bought 5 years
> ago, looks just like the right pix but without the usb connector,
> straight wire into it. Despite many repeated attempts to adjust it, has
> never come within 20 thou of making a repeatable finding. The plastic by
> now is cracked like a century old china bowl and was already crazed when
> it was shipped. Worthless when I paid nearly $200 for it several years
> ago, and still worthless at whatever it is selling for today. I left an
> unfavorable review and was threatened with a lawsuit for libel.
>
> Cheers, Gene Heskett.
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author, 1940)
> If we desire respect for the law, we must first make the law respectable.
>  - Louis D. Brandeis
> Genes Web page 
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[John Dammeyer]

Well that was an interesting read.  I've ordered one of the inexpensive touch 
probes.  Too bad development seems to have stopped 3 years ago.

I installed this on my lab bench Pi4 with LinuxCNC and MESA 7i92H.  I have a 
wire simulating the probe to one of the inputs.  If I start a search motion and 
tap the wire to ground I'll either get a position or a message that it closed 
before it was supposed to or I was too late and probe response not found.

So the hardware is working.  And I'm having the same problem a few people on 
the that forum list were having where none of the local probe screen  jog keys 
work on my AXIS implementation.

I'll continue this discussion on that forum.
John
 

> -Original Message-
> From: andy pugh [mailto:bodge...@gmail.com]
> Sent: October-24-21 7:57 AM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Probing
> 
> On Sun, 24 Oct 2021 at 08:02, John Dammeyer  wrote:
> >
> > Is anyone using
> > https://github.com/verser-git/probe_screen_v2
> >
> > Any comments about it?
> 
> About 50 pages of comments here:
> https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-probe?start=0
> 
> Verser also sells relatively inexpensive touch-probes:
> https://vers.by/en/16-touch-probes
> 
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is
> designed for the especial use of mechanical geniuses, daredevils and
> lunatics."
> � George Fitch, Atlanta Constitution Newspaper, 1912
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[John Dammeyer]

> > I have found this one accurate enough for my needs for manual set up
> > where I move the axis, given the ACME lead screws on my machine.  I
> > have however ordered one of the verser ones (plus extra probes) since
> > it also handles Z and appears to have a bit more 'flex' to deal with
> > deceleration of the axis once the probe makes contact.
> >
> First time I've seen that one which I assume is xy only, but that's also
> a quite decent price. They need to advertise where DDG picks it up. 

The round part is 0.2" diameter.  That dimension is programmed into my 
Shumatech DRO although for the center of a circle, for example it doesn't 
matter.  I touch off in one direction and when the LED comes on zero the X on 
the Shumatech.  Then jog over or use the MPG to move in the other direction 
until the LED comes on again.  At this point FCN, 1, X-Axis buttons.  Now the 0 
position of the X is midway between the two edges.  

Move to that  and do the same but FCN, 1, Y to set the Y axis and now I have 
the center of the circle.  Assuming I have my backlash set perfectly...

I believe the G38.x can be used for this but it requires those macros or chunks 
of G code to set everything.  Hence my original question about probing.  And of 
course I'd have to connect a wire from the probe to the LinuxCNC system since 
it can't look at the LED inside the probe.

John


 But
> I'm so used to a direct electrical contact now that I probably will
> never go back to touch probes. You would laugh at my most used probe,
> its a 3/4" rod of teflon, with a hole bored in the end to accept a piece
> of 12 gauge copper wire which is glued in. A piece of stranded wire
> about 14 gauge, is striped, divided into two, straddles the 12 ga wire
> and is twisted at the far ends to get a grip and contact, drapped over
> something on the head so it doesn't crawl down the wire when I start the
> spindle. The 12 ga, while spinning, is a perfect circle of a size that
> doesn't care as long as its circle is smaller than the hole whose
> location I am probing for. The math in the 4 way probe routine returns
> the exact center of the hole which then becomes the xy touch off point
> with a .0002" max error plus the slop in the ball screws.
> 
> Plenty close enough for the girls I go with at my age. :o)
> 
> Take care John
> 
> Cheers, Gene Heskett.
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author, 1940)
> If we desire respect for the law, we must first make the law respectable.
>  - Louis D. Brandeis
> Genes Web page 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Gene Heskett]

On Sunday 24 October 2021 13:35:17 John Dammeyer wrote:

> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> >
> > On Sunday 24 October 2021 11:30:07 Feral Engineer wrote:
> > > I use work with probe, but I am going to customize the routines a
> > > little to work the way I want them to and Andrew Beck I believe
> > > uses his probes.
> > >
> > > Phil T.
> > >
> > > On Sun, Oct 24, 2021, 11:01 AM andy pugh  
wrote:
> > > > On Sun, 24 Oct 2021 at 08:02, John Dammeyer
> > > > 
> > > >
> > > > wrote:
> > > > > Is anyone using
> > > > > https://github.com/verser-git/probe_screen_v2
> > > > >
> > > > > Any comments about it?
> > > >
> > > > About 50 pages of comments here:
> > > >
> > > > https://forum.linuxcnc.org/49-basic-configuration/29187-work-wit
> > > >h-pr obe?start=0
> > > >
> > > > Verser also sells relatively inexpensive touch-probes:
> > > > https://vers.by/en/16-touch-probes
> >
> > I don't think its a verser product, but the plastic one I bought 5
> > years ago, looks just like the right pix but without the usb
> > connector, straight wire into it. Despite many repeated attempts to
> > adjust it, has never come within 20 thou of making a repeatable
> > finding. The plastic by now is cracked like a century old china bowl
> > and was already crazed when it was shipped. Worthless when I paid
> > nearly $200 for it several years ago, and still worthless at
> > whatever it is selling for today. I left an unfavorable review and
> > was threatened with a lawsuit for libel.
> >
> > Cheers, Gene Heskett.
>
> I broke one of these
> https://www.mscdirect.com/product/details/65002206
> when I accidentally dropped my pendant as I was putting it back on the
> side of the machine (magnets).  The axis selection was still set to X
> and when it dropped it spun the hand wheel fast enough to shift the X
> axis table into the probe tip.  Never did find the probe tip...
>
> I ordered a replacement and now before I hang up the pendant I switch
> the axis selection to off.
>
> I have found this one accurate enough for my needs for manual set up
> where I move the axis, given the ACME lead screws on my machine.  I
> have however ordered one of the verser ones (plus extra probes) since
> it also handles Z and appears to have a bit more 'flex' to deal with
> deceleration of the axis once the probe makes contact.
>
First time I've seen that one which I assume is xy only, but that's also 
a quite decent price. They need to advertise where DDG picks it up.  But 
I'm so used to a direct electrical contact now that I probably will 
never go back to touch probes. You would laugh at my most used probe, 
its a 3/4" rod of teflon, with a hole bored in the end to accept a piece 
of 12 gauge copper wire which is glued in. A piece of stranded wire 
about 14 gauge, is striped, divided into two, straddles the 12 ga wire 
and is twisted at the far ends to get a grip and contact, drapped over 
something on the head so it doesn't crawl down the wire when I start the 
spindle. The 12 ga, while spinning, is a perfect circle of a size that 
doesn't care as long as its circle is smaller than the hole whose 
location I am probing for. The math in the 4 way probe routine returns 
the exact center of the hole which then becomes the xy touch off point 
with a .0002" max error plus the slop in the ball screws.

Plenty close enough for the girls I go with at my age. :o) 

Take care John

Cheers, Gene Heskett.
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[John Dammeyer]

Thanks Andy,
I'm on page 9 of 49.  Will take a bit more time to read all of it.
Sorry to hear about your loss of the probe. Had to be painful.
John


> -Original Message-
> From: andy pugh [mailto:bodge...@gmail.com]
> Sent: October-24-21 7:57 AM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Probing
> 
> On Sun, 24 Oct 2021 at 08:02, John Dammeyer  wrote:
> >
> > Is anyone using
> > https://github.com/verser-git/probe_screen_v2
> >
> > Any comments about it?
> 
> About 50 pages of comments here:
> https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-probe?start=0
> 
> Verser also sells relatively inexpensive touch-probes:
> https://vers.by/en/16-touch-probes
> 
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is
> designed for the especial use of mechanical geniuses, daredevils and
> lunatics."
> � George Fitch, Atlanta Constitution Newspaper, 1912
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[John Dammeyer]

> From: Gene Heskett [mailto:ghesk...@shentel.net]
> 
> On Sunday 24 October 2021 11:30:07 Feral Engineer wrote:
> 
> > I use work with probe, but I am going to customize the routines a
> > little to work the way I want them to and Andrew Beck I believe uses
> > his probes.
> >
> > Phil T.
> > On Sun, Oct 24, 2021, 11:01 AM andy pugh  wrote:
> > > On Sun, 24 Oct 2021 at 08:02, John Dammeyer 
> > >
> > > wrote:
> > > > Is anyone using
> > > > https://github.com/verser-git/probe_screen_v2
> > > >
> > > > Any comments about it?
> > >
> > > About 50 pages of comments here:
> > >
> > > https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-pr
> > >obe?start=0
> > >
> > > Verser also sells relatively inexpensive touch-probes:
> > > https://vers.by/en/16-touch-probes
> 
> I don't think its a verser product, but the plastic one I bought 5 years
> ago, looks just like the right pix but without the usb connector,
> straight wire into it. Despite many repeated attempts to adjust it, has
> never come within 20 thou of making a repeatable finding. The plastic by
> now is cracked like a century old china bowl and was already crazed when
> it was shipped. Worthless when I paid nearly $200 for it several years
> ago, and still worthless at whatever it is selling for today. I left an
> unfavorable review and was threatened with a lawsuit for libel.
> 
> Cheers, Gene Heskett.

I broke one of these 
https://www.mscdirect.com/product/details/65002206
when I accidentally dropped my pendant as I was putting it back on the side of 
the machine (magnets).  The axis selection was still set to X and when it 
dropped it spun the hand wheel fast enough to shift the X axis table into the 
probe tip.  Never did find the probe tip...

I ordered a replacement and now before I hang up the pendant I switch the axis 
selection to off.

I have found this one accurate enough for my needs for manual set up where I 
move the axis, given the ACME lead screws on my machine.  I have however 
ordered one of the verser ones (plus extra probes) since it also handles Z and 
appears to have a bit more 'flex' to deal with deceleration of the axis once 
the probe makes contact.

John





___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Gene Heskett]

On Sunday 24 October 2021 11:30:07 Feral Engineer wrote:

> I use work with probe, but I am going to customize the routines a
> little to work the way I want them to and Andrew Beck I believe uses
> his probes.
>
> Phil T.
> The Feral Engineer
>
> Check out my LinuxCNC tutorials, machine builds and other antics at
> www.youtube.com/c/theferalengineer
>
> Help support my channel efforts and coffee addiction:
> www.patreon.com/theferalengineer
>
> On Sun, Oct 24, 2021, 11:01 AM andy pugh  wrote:
> > On Sun, 24 Oct 2021 at 08:02, John Dammeyer 
> >
> > wrote:
> > > Is anyone using
> > > https://github.com/verser-git/probe_screen_v2
> > >
> > > Any comments about it?
> >
> > About 50 pages of comments here:
> >
> > https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-pr
> >obe?start=0
> >
> > Verser also sells relatively inexpensive touch-probes:
> > https://vers.by/en/16-touch-probes

I don't think its a verser product, but the plastic one I bought 5 years 
ago, looks just like the right pix but without the usb connector, 
straight wire into it. Despite many repeated attempts to adjust it, has 
never come within 20 thou of making a repeatable finding. The plastic by 
now is cracked like a century old china bowl and was already crazed when 
it was shipped. Worthless when I paid nearly $200 for it several years 
ago, and still worthless at whatever it is selling for today. I left an 
unfavorable review and was threatened with a lawsuit for libel.

Cheers, Gene Heskett.
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Feral Engineer]

I use work with probe, but I am going to customize the routines a little to
work the way I want them to and Andrew Beck I believe uses his probes.

Phil T.
The Feral Engineer

Check out my LinuxCNC tutorials, machine builds and other antics at
www.youtube.com/c/theferalengineer

Help support my channel efforts and coffee addiction:
www.patreon.com/theferalengineer

On Sun, Oct 24, 2021, 11:01 AM andy pugh  wrote:

> On Sun, 24 Oct 2021 at 08:02, John Dammeyer 
> wrote:
> >
> > Is anyone using
> > https://github.com/verser-git/probe_screen_v2
> >
> > Any comments about it?
>
> About 50 pages of comments here:
>
> https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-probe?start=0
>
> Verser also sells relatively inexpensive touch-probes:
> https://vers.by/en/16-touch-probes
>
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is
> designed for the especial use of mechanical geniuses, daredevils and
> lunatics."
> — George Fitch, Atlanta Constitution Newspaper, 1912
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[andy pugh]

On Sun, 24 Oct 2021 at 08:02, John Dammeyer  wrote:
>
> Is anyone using
> https://github.com/verser-git/probe_screen_v2
>
> Any comments about it?

About 50 pages of comments here:
https://forum.linuxcnc.org/49-basic-configuration/29187-work-with-probe?start=0

Verser also sells relatively inexpensive touch-probes:
https://vers.by/en/16-touch-probes

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Gene Heskett]

On Sunday 24 October 2021 02:57:39 John Dammeyer wrote:

> Is anyone using
> https://github.com/verser-git/probe_screen_v2
>
Looks neat, but I wrote my own routines for probing years ago that I've 
since made into subroutines I can use anyplace in other programs.  So no 
need for anything quite so elaborate graphicly. As for workpiece 
missmount rotations I use the align kits pieces with my own pyvcp 
buttons to set or cancel the coords corrections.

Looks like it would need some mods today to account for multiple 
spindles. Its old code in that regard.

> Any comments about it?  Or perhaps other Probe installations?

I have never used a 10k spindle speed. 500 revs maybe, but I use a 
capacitor across the probe connection to store the first contact long 
enough to register with linuxcnc, and I probably move slower such that 
the spin only moves .0001" per rotation, giving me .0002" repeatability.
when probing Z, I use a bit of pcb as a live contact, turning the spindle 
backwards with the mill in the spindle serving as the ground. I can use 
the same bit of pcb for weeks without making a visible contact on the 
pcb.

This is cute, it would impress the visiting frogs, but I won't change how 
I do it to this. OLd habits I guess.

> Thanks
> John
>
>
> "ELS! Nothing else works as well for your Lathe"
> Automation Artisans Inc.
> www dot autoartisans dot com
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett.
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Gene Heskett]

On Saturday 08 February 2020 06:24:43 Les Newell wrote:

> The big problem with scanning photographs is distortion. Even with a
> good lens it is surprising how much distortion you get.
>
> Les
>
Which is why I went to extremes to get the camera mounted such that there 
was not any parallax when z was moved. But today those tiny endoscope 
cameras are gone from the market place and I was not able to make 
camview work at all image scalings.  Finding a camera that Just Worked 
turned out to be a very frustrating effort, I probably wasted $500 
trying. And it wasn't the camera as it still worked with cheese by 
shutting lcnc down.  But once it had black screened in camview, it took 
a system reboot to restore its image in camview. And no help from the 
python folks here. A python guru I am not, I can't even play one on tv. 
So I've not fooled with it in a couple years now. The camera plugged in 
right now works, but its not mountable unless you'd say a 5x7 speed 
graphic was mountable. Its physically way to big.


  
> On 07/02/2020 23:42, Greg Bernard wrote:
> > That is interesting and useful, but I wonder if probing the
> > important features and simply tracing a scan or a photograph of the
> > profile in CAD would be quicker and easier for that particular part.
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Les Newell]

The big problem with scanning photographs is distortion. Even with a 
good lens it is surprising how much distortion you get.


Les

On 07/02/2020 23:42, Greg Bernard wrote:

That is interesting and useful, but I wonder if probing the important
features and simply tracing a scan or a photograph of the profile in CAD
would be quicker and easier for that particular part.




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Andy Pugh]

> On 8 Feb 2020, at 08:52, Brent Loschen  wrote:
> 
> When I saw the video, I couldn't help but wonder if there isn't a faster way 
> to probe yet still maintain accuracy.

Almost certainly, but this isn’t something I do every day, so 15 minutes is 
perfectly fine. 

In fact the pay-back time on an improved approach is probably several lifetimes 
:-)



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Brent Loschen]

On 2/7/2020 5:31 PM, Andy Pugh wrote:



On 7 Feb 2020, at 23:45, Greg Bernard  wrote:

That is interesting and useful, but I wonder if probing the important
features and simply tracing a scan or a photograph of the profile in CAD
would be quicker and easier for that particular part.

Possibly, but at least this way it is definitely scaled in mm, and furthermore 
the same mm as my mill.



I either do a direct scan of the part, or trace on paper then scan, and 
bring the bitmap into Inkscape.    From there I convert it to svg, and 
let Inkscape find the edges, save the profile as a dxf, and bring that 
into CAD.  It's usually easy to get < .5mm accuracy. With extra care and 
some tweaking in Inscape it's not impossible to hit .25 - .30 mm edge to 
edge accuracy, especially from a direct scan.  If the part is scan-able, 
it also works for locating holes and pockets.  Large parts can be 
scanned in sections and stitched together in the tool.  Unfortunately , 
even .25 isn't good enough for some applications.


When I saw the video, I couldn't help but wonder if there isn't a faster 
way to probe yet still maintain accuracy.  I thought about a hybrid 
approach, where you take that profile from Inkscape and feed it to a 
routine that probes the actual part, but now from within a 1-2mm 
envelope of the provided profile.  If the profile has long straight 
edges, the routine need only probe the beginning and the end of that 
line.   "Smart probing"! Just a thought.



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Andy Pugh]

> On 7 Feb 2020, at 23:45, Greg Bernard  wrote:
> 
> That is interesting and useful, but I wonder if probing the important
> features and simply tracing a scan or a photograph of the profile in CAD
> would be quicker and easier for that particular part.

Possibly, but at least this way it is definitely scaled in mm, and furthermore 
the same mm as my mill. 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Greg Bernard]

That is interesting and useful, but I wonder if probing the important
features and simply tracing a scan or a photograph of the profile in CAD
would be quicker and easier for that particular part.

On Fri, Feb 7, 2020 at 11:25 AM John Dammeyer 
wrote:

> Pretty cool.
> John
>
>
> > -Original Message-
> > From: andy pugh [mailto:bodge...@gmail.com]
> > Sent: February-07-20 1:59 AM
> > To: Enhanced Machine Controller (EMC)
> > Subject: Re: [Emc-users] Probing a Profile
> >
> > On Wed, 5 Feb 2020 at 23:52, andy pugh  wrote:
> >
> > > And here is the G-code routine I used.
> >
> > Which is usable, but slightly flawed, in that if the probe _just_
> > catches a corner, the retract distance means that the "i missed"
> > circle can miss the work.
> > So a slight re-think needed there.
> >
> > I made a video of the process, showing how at one corner I needed to
> > poke the probe by hand to get it to find the work.
> > https://www.youtube.com/watch?v=JO8lLaV6pbw
> >
> > I have also just realised that there is a fairly easy way to auto stop
> > using the well-known concept of "winding number" which #1 is
> > accidentally calculating
> > https://en.wikipedia.org/wiki/Point_in_polygon#Winding_number_algorith
> > m
> >
> > Rather than O100 WHILE [#<_flood> EQ 0] (use the flood button to stop
> > and save data)
> >
> > I could use O100 WHILE [#1 < 361]
> >
> > --
> > atp
> > "A motorcycle is a bicycle with a pandemonium attachment and is
> > designed for the especial use of mechanical geniuses, daredevils and
> > lunatics."
> > � George Fitch, Atlanta Constitution Newspaper, 1912
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>


-- 
"Anyone who believes exponential growth can go on forever in a finite world
is either a madman or an economist."
-Kenneth Boulding, economist
Corporations are NOT people and money is NOT speech!

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[John Dammeyer]

Pretty cool.
John


> -Original Message-
> From: andy pugh [mailto:bodge...@gmail.com]
> Sent: February-07-20 1:59 AM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Probing a Profile
> 
> On Wed, 5 Feb 2020 at 23:52, andy pugh  wrote:
> 
> > And here is the G-code routine I used.
> 
> Which is usable, but slightly flawed, in that if the probe _just_
> catches a corner, the retract distance means that the "i missed"
> circle can miss the work.
> So a slight re-think needed there.
> 
> I made a video of the process, showing how at one corner I needed to
> poke the probe by hand to get it to find the work.
> https://www.youtube.com/watch?v=JO8lLaV6pbw
> 
> I have also just realised that there is a fairly easy way to auto stop
> using the well-known concept of "winding number" which #1 is
> accidentally calculating
> https://en.wikipedia.org/wiki/Point_in_polygon#Winding_number_algorith
> m
> 
> Rather than O100 WHILE [#<_flood> EQ 0] (use the flood button to stop
> and save data)
> 
> I could use O100 WHILE [#1 < 361]
> 
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is
> designed for the especial use of mechanical geniuses, daredevils and
> lunatics."
> � George Fitch, Atlanta Constitution Newspaper, 1912
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[andy pugh]

On Wed, 5 Feb 2020 at 23:52, andy pugh  wrote:

> And here is the G-code routine I used.

Which is usable, but slightly flawed, in that if the probe _just_
catches a corner, the retract distance means that the "i missed"
circle can miss the work.
So a slight re-think needed there.

I made a video of the process, showing how at one corner I needed to
poke the probe by hand to get it to find the work.
https://www.youtube.com/watch?v=JO8lLaV6pbw

I have also just realised that there is a fairly easy way to auto stop
using the well-known concept of "winding number" which #1 is
accidentally calculating
https://en.wikipedia.org/wiki/Point_in_polygon#Winding_number_algorithm

Rather than O100 WHILE [#<_flood> EQ 0] (use the flood button to stop
and save data)

I could use O100 WHILE [#1 < 361]

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[andy pugh]

On Tue, 4 Feb 2020 at 21:25, Todd Zuercher  wrote:

> To deal with probe tip, probe the perimeter, connect the dots, then just 
> offset the shape you made with the probe's tip radius.

That works a treat once the points are in the CAD.

And here is the G-code routine I used.

;probe a profile
;the routine will initially probe in negative Y and will walk around
the profile clockwise
;but can follow a re-entrant shape

#1 = 0 (explore angle)
#2 = #<_X> (start positions)
#3 = #<_Y>
#4 = 3 (step size)
#5 = 0.5 (retract on sucessful probe)
(AXIS,stop)
(LOGOPEN,profile1.txt)
O100 WHILE [#<_flood> EQ 0] (use the flood button to stop and save data)
G38.3 F100 X[#2 + #4 * COS[#1 - 90]] Y[#3 + #4 * SIN[#1 - 90]]
O101 IF [#5070 EQ 1]
G38.5 F20 X#2 Y#3 (slow probe away, store point)

(LOG, #5061 #5062)

#2 = [#5061 + #5 * COS[#1 + 90]]
#3 = [#5062 + #5 * SIN[#1 + 90]]
G0 X#2 Y#3 (1mm back along probe track)
O102 DO
G38.5 F500 X#2 Y#3
G38.3 F500 X[#2 + #4 * COS[#1]] Y[#3 + #4 * SIN[#1]]
O103 IF [#5070 EQ 1]
#1 = [#1 + 15]
O103 ENDIF
O102 WHILE [#5070 EQ 1]
#2 = #<_X>
#3 = #<_Y>
O101 ELSE
(missed, so now start a clockwise polygon looking for the edge)
#1 = [#1 - 15]
O101 ENDIF
O100 ENDWHILE
(LOGCLOSE)
M2


-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile --> Coordinate measurement machine

[Eric Keller]

I have programmed a cmm, but I really don't remember anything about it.
Rapid moves are like g code, but I think the one I used had a probe command.


On Wed, Feb 5, 2020 at 1:00 PM N  wrote:

> Anyone used a coordinate measurement machine and know how they do?
>
> Maybe I happen to have manual but will probably not have to much time to
> look into it this week.
>
> > I think it comes down to constructing lines perp to the profile at
> > probed points. CMM's obviously take care of this somehow.
> >
> > I've done it the hard way by drawing circles the diameter of the probe
> > and then doing three pt arcs to fit. Certainly there are better and
> > considerably more elegant ways to do this. What I can visualize in
> > concept I cannot convert to good calculations. ;-)  I passed calculus
> > but knew better than to try dif-e-q. A second order curve fit tangent to
> > multiple circles might be a better approach.
> >
> > "Implementation is left as an exercise for the student."  :-)
> >
> > Dave
> >
> > On 2/4/20 3:57 AM, andy pugh wrote:
> > > Does anyone have a G-code routine to probe around a profile to trace
> it out?
> > >
> > > I imagine some sort of "keep turning right" algorithm should be able
> > > to walk round a profile, though exactly how you compensate for probe
> > > diameter on external corners has me a bit stumped.
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile --> Coordinate measurement machine

[N]

Anyone used a coordinate measurement machine and know how they do?

Maybe I happen to have manual but will probably not have to much time to look 
into it this week.

> I think it comes down to constructing lines perp to the profile at 
> probed points. CMM's obviously take care of this somehow.
> 
> I've done it the hard way by drawing circles the diameter of the probe 
> and then doing three pt arcs to fit. Certainly there are better and 
> considerably more elegant ways to do this. What I can visualize in 
> concept I cannot convert to good calculations. ;-)  I passed calculus 
> but knew better than to try dif-e-q. A second order curve fit tangent to 
> multiple circles might be a better approach.
> 
> "Implementation is left as an exercise for the student."  :-)
> 
> Dave
> 
> On 2/4/20 3:57 AM, andy pugh wrote:
> > Does anyone have a G-code routine to probe around a profile to trace it out?
> >
> > I imagine some sort of "keep turning right" algorithm should be able
> > to walk round a profile, though exactly how you compensate for probe
> > diameter on external corners has me a bit stumped.


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Todd Zuercher]

To deal with probe tip, probe the perimeter, connect the dots, then just offset 
the shape you made with the probe's tip radius.

Todd Zuercher
P. Graham Dunn Inc.
630 Henry Street 
Dalton, Ohio 44618
Phone:  (330)828-2105ext. 2031

-Original Message-
From: andy pugh  
Sent: Tuesday, February 04, 2020 12:31 PM
To: Enhanced Machine Controller (EMC) 
Subject: Re: [Emc-users] Probing a Profile

[EXTERNAL EMAIL] Be sure links are safe.

On Tue, 4 Feb 2020 at 16:22, dave engvall  wrote:

> I've done it the hard way by drawing circles the diameter of the probe

I can handle that, at a push. But what did you use to control the probing 
process?

--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is designed for 
the especial use of mechanical geniuses, daredevils and lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[dave engvall]

Been so long I don't remember. I was done on the Mazak so it has been a 
few years. I probably wrote something rather simple. Maybe even so 
simplistic and manual. ;-)


Dave

On 2/4/20 9:31 AM, andy pugh wrote:

On Tue, 4 Feb 2020 at 16:22, dave engvall  wrote:


I've done it the hard way by drawing circles the diameter of the probe

I can handle that, at a push. But what did you use to control the
probing process?




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[Gene Heskett]

On Tuesday 04 February 2020 06:57:54 andy pugh wrote:

> Does anyone have a G-code routine to probe around a profile to trace
> it out?
>
> I imagine some sort of "keep turning right" algorithm should be able
> to walk round a profile, though exactly how you compensate for probe
> diameter on external corners has me a bit stumped.

A reasonably accurate measurement would be to subtract the probes tip 
radii when the last samples are a straight line and when arriving at a 
corner do the subtractions using sin and cos of the new readings, 
scaling the radii accordingly. The problem there is how far does the 
probe move to open the contacts. Probably done more accurately with a 
camera with only 4 pixels unless you have a very sensitive probe.  I 
think I'd druther use a contact probe as it would have less flex. A bit 
of wobble would make contact and lose it, allowing the angle of the 
surface to be detected well enough to steer the contact search. but 
would limit the rpm and search speeds, to the point of impractical time 
wise. It could be done, but might take 3 weeks.

I once scanned the floor plate of my P-17 to a 20 thou grid, looked 
pretty good but took nearly 2 weeks and was only one side of it. I had 
visions of making a alu version. I also had contact reliability problems 
be cause of the parkerized finish in it. Gave up. I very briefly 
considered takeing the profile of the new SS 6.5 barrel I was about to 
put on old meat in the pot, then sanding it down to about half ifs 
weight and rewraping it in carbon fiber to about the same profile, but 
the cost of the fiber and the resin's environmental aspects brought me 
to my senses, not to mention the time for the invention of the tool post 
to apply the resin and wind the fiber in a nice artistic x pattern.  
Nice idea on the face of it, but I'd have had 5x its $650 cost in it by 
the time I was ready to put it in the barrel vice and screw it in. It 
shoots well but that SS is heavy, too heavy for carrying around in the 
deer woods at my age.  To/from a well placed and camo'd blind might be 
doable though. Finding a place to put that blind is another project 
entirely.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[andy pugh]

On Tue, 4 Feb 2020 at 16:22, dave engvall  wrote:

> I've done it the hard way by drawing circles the diameter of the probe

I can handle that, at a push. But what did you use to control the
probing process?

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing a Profile

[dave engvall]

I think it comes down to constructing lines perp to the profile at 
probed points. CMM's obviously take care of this somehow.


I've done it the hard way by drawing circles the diameter of the probe 
and then doing three pt arcs to fit. Certainly there are better and 
considerably more elegant ways to do this. What I can visualize in 
concept I cannot convert to good calculations. ;-)  I passed calculus 
but knew better than to try dif-e-q. A second order curve fit tangent to 
multiple circles might be a better approach.


"Implementation is left as an exercise for the student."  :-)

Dave

On 2/4/20 3:57 AM, andy pugh wrote:

Does anyone have a G-code routine to probe around a profile to trace it out?

I imagine some sort of "keep turning right" algorithm should be able
to walk round a profile, though exactly how you compensate for probe
diameter on external corners has me a bit stumped.




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[gene heskett]

On Tuesday, January 31, 2012 11:15:31 AM Chris Radek did opine:

 On Tue, Jan 31, 2012 at 10:49:04AM -0500, gene heskett wrote:
  show stopper.  In doing a G38.2 f1 z2.5, it will probably stop well
  within a thou of contact.  But then I am dead in the water because
  when I try to do a z move to #5063 + 0.01, it will move about .0005,
  breaking the contact, which is then reported as an error, shutting
  the machine down and
 
 Exactly what error do you get?
 
 I'm suspicious that it's not the break that's the error, it's
 another bounced make.

While that is virtually guaranteed to happen Chris, my point is that once 
the G38.2 move has detected a closure, stopped the named axis and recorded 
the machine state, the usefulness of the probe has been fulfilled, so why 
the heck should it care one way or the other when the machine tries to do a 
g0 z[#5063 +0.02] in order to back off and retry the G38.2 with a much 
smaller Fspeed to get a fine tuned position that doesn't have as much 
overshoot it it due to the machines stopping distances.  It shouldn't care 
about the probe status when its making a non-probe related move.  It does 
care while executing the following G00 or G01 move, and its reporting the 
probe break error down in the lower right corner and aborting the program.

One thought I just had was to kill the move blending by a G34? P1 as the 
next move, forcing a full dead stop after the G38.2.  I'll do that in an 
hour or so and see if that fixes it.

Cheers, Gene
-- 
There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order.
-Ed Howdershelt (Author)
My web page: http://coyoteden.dyndns-free.com:85/gene
Is your job running?  You'd better go catch it!

--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[Erik Friesen]

Could there be any connection with this to the M66 problem I have listed
herehttp://sourceforge.net/tracker/?func=detailatid=106744aid=3477158group_id=6744?

I think its an error in communication between the top and bottom levels.
If M66 is followed by an oname etc,  the decoder sees this as two subs
with the same name, the second time around.

My apologies if this has no bearing on the issue.

On Tue, Jan 31, 2012 at 11:13 AM, Chris Radek ch...@timeguy.com wrote:

 On Tue, Jan 31, 2012 at 10:49:04AM -0500, gene heskett wrote:
 
  show stopper.  In doing a G38.2 f1 z2.5, it will probably stop well
 within
  a thou of contact.  But then I am dead in the water because when I try to
  do a z move to #5063 + 0.01, it will move about .0005, breaking the
  contact, which is then reported as an error, shutting the machine down
 and

 Exactly what error do you get?

 I'm suspicious that it's not the break that's the error, it's
 another bounced make.



 --
 Keep Your Developer Skills Current with LearnDevNow!
 The most comprehensive online learning library for Microsoft developers
 is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
 Metro Style Apps, more. Free future releases when you subscribe now!
 http://p.sf.net/sfu/learndevnow-d2d
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users

--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[Chris Radek]

On Tue, Jan 31, 2012 at 11:31:26AM -0500, gene heskett wrote:

 the machine state, the usefulness of the probe has been fulfilled, so why 
 the heck should it care one way or the other when the machine tries to do a 
 g0 z[#5063 +0.02] in order to back off 

I sympathize with you being frustrated with this, but the reason for a
probe RISING edge during a machine rapid causing the machine to stop
is very clear - if you don't mean to be probing, and you're rapiding,
and something hits the probe, the next half-second or so may cause the
shedding of many tears and dollars if the machine doesn't stop.  Those
things are shockingly expensive.

Problems with bounce are a pain though, and not just for linuxcnc
users I bet, because my Renishaw has a debounce time constant, in the
hardware, of several ms.  I do final probe moves (length of only about
.002) at F0.1!

 It does 
 care while executing the following G00 or G01 move, and its reporting the 
 probe break error down in the lower right corner and aborting the program.

Ok you're saying probe BREAK error again here, and I wonder if that's
really the error you're getting.  Can you say what the exact error
message is please?

I think it must be one of these?

reportError(_(Probe tripped during non-probe MDI command.));
reportError(_(Probe tripped during homing motion.));
reportError(_(Probe tripped during a jog.));

There are also

reportError(_(G38.4 move finished without breaking contact.));
reportError(_(G38.2 move finished without making contact.));

which is the only place I can find break in an error message, but if
you're not in a probing move when it happens, it won't be these.

Also are you running in auto mode, or are you using MDI to do this?  I
think it's more forgiving in auto mode but I'd have to study/remember
harder to be sure.

--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[Peter C. Wallace]

On Tue, 31 Jan 2012, gene heskett wrote:

 Date: Tue, 31 Jan 2012 11:31:26 -0500
 From: gene heskett ghesk...@wdtv.com
 Reply-To: Enhanced Machine Controller (EMC)
 emc-users@lists.sourceforge.net
 To: emc-users@lists.sourceforge.net
 Subject: Re: [Emc-users] Probing error?
 
 On Tuesday, January 31, 2012 11:15:31 AM Chris Radek did opine:

 On Tue, Jan 31, 2012 at 10:49:04AM -0500, gene heskett wrote:
 show stopper.  In doing a G38.2 f1 z2.5, it will probably stop well
 within a thou of contact.  But then I am dead in the water because
 when I try to do a z move to #5063 + 0.01, it will move about .0005,
 breaking the contact, which is then reported as an error, shutting
 the machine down and

 Exactly what error do you get?

 I'm suspicious that it's not the break that's the error, it's
 another bounced make.

 While that is virtually guaranteed to happen Chris, my point is that once
 the G38.2 move has detected a closure, stopped the named axis and recorded
 the machine state, the usefulness of the probe has been fulfilled, so why
 the heck should it care one way or the other when the machine tries to do a
 g0 z[#5063 +0.02] in order to back off and retry the G38.2 with a much
 smaller Fspeed to get a fine tuned position that doesn't have as much
 overshoot it it due to the machines stopping distances.  It shouldn't care
 about the probe status when its making a non-probe related move.  It does
 care while executing the following G00 or G01 move, and its reporting the
 probe break error down in the lower right corner and aborting the program.

 One thought I just had was to kill the move blending by a G34? P1 as the
 next move, forcing a full dead stop after the G38.2.  I'll do that in an
 hour or so and see if that fixes it.

 Cheers, Gene
 -- 
 There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order.
 -Ed Howdershelt (Author)
 My web page: http://coyoteden.dyndns-free.com:85/gene
 Is your job running?  You'd better go catch it!


Could this be fixed by a simple RC bounce filter followed by a
Schmitt trigger?

(or maybe the software debounce comp in series with probe input)


Peter Wallace
Mesa Electronics

(\__/)
(='.'=) This is Bunny. Copy and paste bunny into your
()_() signature to help him gain world domination.


--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[gene heskett]

On Tuesday, January 31, 2012 06:57:39 PM Chris Radek did opine:

 On Tue, Jan 31, 2012 at 11:31:26AM -0500, gene heskett wrote:
  the machine state, the usefulness of the probe has been fulfilled, so
  why the heck should it care one way or the other when the machine
  tries to do a g0 z[#5063 +0.02] in order to back off
 
 I sympathize with you being frustrated with this, but the reason for a
 probe RISING edge during a machine rapid causing the machine to stop
 is very clear - if you don't mean to be probing, and you're rapiding,
 and something hits the probe, the next half-second or so may cause the
 shedding of many tears and dollars if the machine doesn't stop.  Those
 things are shockingly expensive.

This could be usable, IF the probe was isolated, but it is not, its the pcb 
material that is isolated.  In this case, any move in the upper hemisphere 
s/b legal.  There is nothing in the up direction but the end of the post or 
the top of the gearbox hitting the Z bearing housing.
 
 Problems with bounce are a pain though, and not just for linuxcnc
 users I bet, because my Renishaw has a debounce time constant, in the
 hardware, of several ms.  I do final probe moves (length of only about
 .002) at F0.1!

I'd have to come from about .0100 up as there is about 5 thou of backlash, 
and my last probe move now is at .5 ipm.  At .1, its so slow you have to 
actually check the Z motor coupling to see if its working at all.
 
  It does
  care while executing the following G00 or G01 move, and its reporting
  the probe break error down in the lower right corner and aborting the
  program.
 
 Ok you're saying probe BREAK error again here, and I wonder if that's
 really the error you're getting.  Can you say what the exact error
 message is please?
 
 I think it must be one of these?
 
 reportError(_(Probe tripped during non-probe MDI command.));
 reportError(_(Probe tripped during homing motion.));
 reportError(_(Probe tripped during a jog.));
 
This last one, when the jog direction is up, but the wording doesn't say 
tripped, it says break.  It would be a heck of a lot easier if the message 
it pops up was capable of being copied and pasted, but none of them are.

But my idea of killing the motion blending with a G04 P1 second pause 
immediately after the G38.2 seems to have fixed that right up, by giving 
the motion queue a chance to drain or whatever its called.

 There are also
 
 reportError(_(G38.4 move finished without breaking contact.));
 reportError(_(G38.2 move finished without making contact.));
 
 which is the only place I can find break in an error message, but if
 you're not in a probing move when it happens, it won't be these.
 
 Also are you running in auto mode, or are you using MDI to do this?  I
 think it's more forgiving in auto mode but I'd have to study/remember
 harder to be sure.

Its a called, named subroutine file.  Running in either MDI or auto mode.

My first board attempt says I'm milling too deep, so how deep do most folks 
go?  Currently set for .003 below the G38.2 contact.  ATM, if I can find 
the end of the first pass in that file I am going to nuke that, set the 
machine zero about .002 higher and do the back side of that same board for 
SG.  Back in a couple hours.

Thanks.

Cheers, Gene
-- 
There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order.
-Ed Howdershelt (Author)
My web page: http://coyoteden.dyndns-free.com:85/gene
They also surf who only stand on waves.

--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[gene heskett]

On Tuesday, January 31, 2012 07:19:33 PM Peter C. Wallace did opine:

 On Tue, 31 Jan 2012, gene heskett wrote:
  Date: Tue, 31 Jan 2012 11:31:26 -0500
  From: gene heskett ghesk...@wdtv.com
  Reply-To: Enhanced Machine Controller (EMC)
  
  emc-users@lists.sourceforge.net
  
  To: emc-users@lists.sourceforge.net
  Subject: Re: [Emc-users] Probing error?
  
  On Tuesday, January 31, 2012 11:15:31 AM Chris Radek did opine:
  On Tue, Jan 31, 2012 at 10:49:04AM -0500, gene heskett wrote:
  show stopper.  In doing a G38.2 f1 z2.5, it will probably stop well
  within a thou of contact.  But then I am dead in the water because
  when I try to do a z move to #5063 + 0.01, it will move about .0005,
  breaking the contact, which is then reported as an error, shutting
  the machine down and
  
  Exactly what error do you get?
  
  I'm suspicious that it's not the break that's the error, it's
  another bounced make.
  
  While that is virtually guaranteed to happen Chris, my point is that
  once the G38.2 move has detected a closure, stopped the named axis
  and recorded the machine state, the usefulness of the probe has been
  fulfilled, so why the heck should it care one way or the other when
  the machine tries to do a g0 z[#5063 +0.02] in order to back off and
  retry the G38.2 with a much smaller Fspeed to get a fine tuned
  position that doesn't have as much overshoot it it due to the
  machines stopping distances.  It shouldn't care about the probe
  status when its making a non-probe related move.  It does care while
  executing the following G00 or G01 move, and its reporting the probe
  break error down in the lower right corner and aborting the program.
  
  One thought I just had was to kill the move blending by a G34? P1 as
  the next move, forcing a full dead stop after the G38.2.  I'll do
  that in an hour or so and see if that fixes it.
  
  Cheers, Gene
 
 Could this be fixed by a simple RC bounce filter followed by a
 Schmitt trigger?
 
 (or maybe the software debounce comp in series with probe input)
 
I thought of that too Peter, but found that a solid 1 second pause 
immediately after the G38.2 had a hit, took care of it.
 
 Peter Wallace
 Mesa Electronics

Thanks Peter.

Cheers, Gene
-- 
There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order.
-Ed Howdershelt (Author)
My web page: http://coyoteden.dyndns-free.com:85/gene
Silvrbear Oxymorons?  I saw one yesterday - the pamphlet on Taco Bell
Nutritional Information

--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing error?

[dave]

On Tue, 31 Jan 2012 19:18:41 -0500
gene heskett ghesk...@wdtv.com wrote:

 On Tuesday, January 31, 2012 06:57:39 PM Chris Radek did opine:
 
  On Tue, Jan 31, 2012 at 11:31:26AM -0500, gene heskett wrote:
   the machine state, the usefulness of the probe has been
   fulfilled, so why the heck should it care one way or the other
   when the machine tries to do a g0 z[#5063 +0.02] in order to back
   off
  
  I sympathize with you being frustrated with this, but the reason
  for a probe RISING edge during a machine rapid causing the machine
  to stop is very clear - if you don't mean to be probing, and you're
  rapiding, and something hits the probe, the next half-second or so
  may cause the shedding of many tears and dollars if the machine
  doesn't stop.  Those things are shockingly expensive.
Yes, they are: but shop-built ones can be quite effective. A couple of
years ago I posted a design for a simple probe ... done with 3 thick
brass buttons isolated by nylon and epoxy and .1875 dowel pins to fit
into the cones on the buttons. Really not good to better than 0.1 thou
in xy plane or z. Still good enough for amateur use. :-)
Someplace in the archives of the usr list are posts and a pointer to
some pics. If you paid $ for a commercial probe the real caution is
in order. 

Dave

 
 This could be usable, IF the probe was isolated, but it is not, its
 the pcb material that is isolated.  In this case, any move in the
 upper hemisphere s/b legal.  There is nothing in the up direction but
 the end of the post or the top of the gearbox hitting the Z bearing
 housing. 
  Problems with bounce are a pain though, and not just for linuxcnc
  users I bet, because my Renishaw has a debounce time constant, in
  the hardware, of several ms.  I do final probe moves (length of
  only about .002) at F0.1!
 
 I'd have to come from about .0100 up as there is about 5 thou of
 backlash, and my last probe move now is at .5 ipm.  At .1, its so
 slow you have to actually check the Z motor coupling to see if its
 working at all. 
   It does
   care while executing the following G00 or G01 move, and its
   reporting the probe break error down in the lower right corner
   and aborting the program.
  
  Ok you're saying probe BREAK error again here, and I wonder if
  that's really the error you're getting.  Can you say what the exact
  error message is please?
  
  I think it must be one of these?
  
  reportError(_(Probe tripped during non-probe MDI command.));
  reportError(_(Probe tripped during homing motion.));
  reportError(_(Probe tripped during a jog.));
  
 This last one, when the jog direction is up, but the wording doesn't
 say tripped, it says break.  It would be a heck of a lot easier if
 the message it pops up was capable of being copied and pasted, but
 none of them are.
 
 But my idea of killing the motion blending with a G04 P1 second pause 
 immediately after the G38.2 seems to have fixed that right up, by
 giving the motion queue a chance to drain or whatever its called.
 
  There are also
  
  reportError(_(G38.4 move finished without breaking contact.));
  reportError(_(G38.2 move finished without making contact.));
  
  which is the only place I can find break in an error message, but
  if you're not in a probing move when it happens, it won't be these.
  
  Also are you running in auto mode, or are you using MDI to do
  this?  I think it's more forgiving in auto mode but I'd have to
  study/remember harder to be sure.
 
 Its a called, named subroutine file.  Running in either MDI or auto
 mode.
 
 My first board attempt says I'm milling too deep, so how deep do most
 folks go?  Currently set for .003 below the G38.2 contact.  ATM, if
 I can find the end of the first pass in that file I am going to nuke
 that, set the machine zero about .002 higher and do the back side of
 that same board for SG.  Back in a couple hours.
 
 Thanks.
 
 Cheers, Gene


--
Keep Your Developer Skills Current with LearnDevNow!
The most comprehensive online learning library for Microsoft developers
is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3,
Metro Style Apps, more. Free future releases when you subscribe now!
http://p.sf.net/sfu/learndevnow-d2d
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing!

[Gene Heskett]

On Monday 07 December 2009, dave wrote:
Hi all,
For once I'm going to crow rather than eat crow.

Discussions with Matt Shaver yielded an idea for a probe that was not
the classical Renishaw ball and bar design.

To wit:
Drill and ream 0.187 holes in a disk on a 2 bolt circle and press
0.1875 ground dowel pins into the hole. Arrange so they protrude
approx .3. Drill a hole in the center of the disk and tap 1/4-28 to
attach the probe. You will note set screws in the pic since I didn't
have an undersize reamer.

Mill holes 0.8 dia in another disk on the same bolt circle.
Make cups in .75 dia x .5 cylinders by drilling with a #2
drill/countersink. Put teflon washers in the holes in disk and float the
cups in epoxy using the dowel pins as a jig to align the cups.
Tap the cups with a 4-40 to attach electrical connections.

The logic utilizes the inverting inputs on a hal logic 3 input OR to
digital inputs on the stg card. A wire off the disk with the pins goes
to digital ground. No pullups were necessary.

see


http://imagebin.ca/view/UHmqcPz.html

Needs one or 2 more pix Dave, one with the probe tip installed, and one of it 
installed one the mill ready to work.  The logic I can get, and using a 3 
input gate certainly simplifies the probe.  Not clear in this pix but I 
assume the pins being held by the set-screws are also brass?  Tip profile?  A 
silver plate kit might make it even more accurate, but this is certainly 
tolerable accuracy indeed. :)

Now for the proof of the pudding.

Used G38.3 probe a ground surface to check Z repeatability. G code was
provided by a C program that simply looped. (PROBEOPEN dataset_name) and
(PROBECLOSE) were used to accumulate the data.
AFIK if one uses a path in the dataset name then spacing between the
PROBEOPEN and the dataset name is not critical; otherwise extra spaces
i.e.  1 will be prepended to the data set name. Ask me how I know. ;-)
For each test reps = 30.

In like manner I probed the bed at 1 intervals and also used movements
in X to probe the side of a ground bar.

Note: resolution of the axes are 1 um in X and Y and about 1.5 um in Z.
  encoders are on the ball screw for X and Y and on the servo motor
for Z.

Results:   std dev.
X probe:   0.00022
Z probe:   0.000267
Bed probe: 0.000634

I think I can live with these numbers for a shop-built probe. ;-)

And they are better than the optical, z only gizmo I made following 
directions from someone here (Matt Shaver?), that seemed to have a 
repeatability of maybe a fat thou.  I had figured to use math to smooth the 
curve if and when I got around to finishing the outside face of the floor 
plate I have about 2//3rds finished for my old Akley-06.  Using a 1/4 ball 
nose, I was going to retrace the map of the old one on about a .005 pass 
increment.  But I've miss laid my round tuit.  The idea was to replace the 
whole magazine well, trigger guard and floor plate with alu parts eventually, 
which would lighten the whole thing by half a pound or more.  As is, it's 
nearly 14 pounds loaded and hanging on my shoulder.  Laminated walnut is 
dense  P14's never were noted for being light by the time a medium heavy 26 
Douglas is screwed into them and a big variable scope mounted.

Many thanks to those hard working (and I might add bright) people that
created the various components that made this this implementation
possible.

Dave

I'll second that.  Loudly.

-- 
Cheers, Gene
There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order.
-Ed Howdershelt (Author)
The NRA is offering FREE Associate memberships to anyone who wants them.
https://www.nrahq.org/nrabonus/accept-membership.asp

How many people work here?
Oh, about half.

--
Join us December 9, 2009 for the Red Hat Virtual Experience,
a free event focused on virtualization and cloud computing. 
Attend in-depth sessions from your desk. Your couch. Anywhere.
http://p.sf.net/sfu/redhat-sfdev2dev
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing Results

[Jeff Epler]

A comment of the form (PROBEOPEN filename.txt) will open filename.txt
and store the 9-number coordinate of each successful straight probe in
it. The file must be closed with (PROBECLOSE).
http://linuxcnc.org/docs/html/gcode_main.html#sub:G38.2:-Straight-Probe

Jeff

--
This SF.net email is sponsored by:
SourcForge Community
SourceForge wants to tell your story.
http://p.sf.net/sfu/sf-spreadtheword
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing Results

[saadp]

Okay, I inserted (PROBEOPEN filename.txt) and (PROBECLOSE) in my program.

EMC2 creates a file in the machine config directory that looks like an array:

-26.931041 -44.450006 5.02 0.00 0.00 0.00 0.00 0.00
0.00

-26.945332 -44.450006 5.02 0.00 0.00 0.00 0.00 0.00
0.00

-29.545331 -44.450006 8.411713 0.00 0.00 0.00 0.00 0.00
0.00

Now I understand why I am getting an unexpected behavior. After probing, I would
like to re-use in my program the values 8.8.411713 and 5.02.

Is there some sort of buffer in EMC2 that stores each individual value?

Regards,
Patrice

--
This SF.net email is sponsored by:
SourcForge Community
SourceForge wants to tell your story.
http://p.sf.net/sfu/sf-spreadtheword
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing Results

[Jeff Epler]

As you showed in your first post, you can save the results of a
probe operation to another numbered parameter, if you want to use it
during the same part program.

The results of (PROBEOPEN) are for processing with some other software
according to the various needs of different users.

If you want to use that number during a different part program, you can
decide on a parameter number to communicate between the two part
programs.  By inserting that number in your .var file along with a dummy
value (edit the .var file only while emc is not open!) the variable will
now be saved from run to run and part program to part program.   Keep
the .var file in order.

If this still doesn't answer your question, please try to be more
specific about what you'd like to do.

Jeff

--
This SF.net email is sponsored by:
SourcForge Community
SourceForge wants to tell your story.
http://p.sf.net/sfu/sf-spreadtheword
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing Results

[saadp]

Thanks Jeff. I got it.

I was not saving the result of the probing operation properly.

I want to use it during the same part program so no need to mess with the var
file.

Best Regards,

Patrice



--
This SF.net email is sponsored by:
SourcForge Community
SourceForge wants to tell your story.
http://p.sf.net/sfu/sf-spreadtheword
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing with a gimbled head.

[Dave Keeton]

Thanks Stuart,
  I have been asked to build a machine that can digitize
complex parts (Landing gear). The catch is that it needs to be a Lights
Out Operation - fully automated. The only way I can see to do this is
with a gimbled head and probe on a custom built machine. Thanks for
looking into it. I think EMC should be able to do this.

  Dave

On Thu, 2008-11-27 at 22:00 -0600, Stuart Stevenson wrote:
 Dave,
As soon as I get the cinci running and comped I will start working
 on the probing.
If you position the gimbaled head and then qualify the probe to a
 standard you will have no issues of accuracy in the gimbaled head. You
 would have access and accuracy.
 
 On Thu, Nov 27, 2008 at 8:50 AM, Dave Keeton [EMAIL PROTECTED] wrote:
  How well does probing and digitizing with a gimbled type spindle work?
  Has any one done this. I would like to use it for digitizing complex
  parts.
 
 Thanks in advance for any ideas offered...
  Dave
 
 
 
  -
  This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
  Build the coolest Linux based applications with Moblin SDK  win great 
  prizes
  Grand prize is a trip for two to an Open Source event anywhere in the world
  http://moblin-contest.org/redirect.php?banner_id=100url=/
  ___
  Emc-users mailing list
  Emc-users@lists.sourceforge.net
  https://lists.sourceforge.net/lists/listinfo/emc-users
 
 
 
 -
 This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
 Build the coolest Linux based applications with Moblin SDK  win great prizes
 Grand prize is a trip for two to an Open Source event anywhere in the world
 http://moblin-contest.org/redirect.php?banner_id=100url=/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users


-
This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
Build the coolest Linux based applications with Moblin SDK  win great prizes
Grand prize is a trip for two to an Open Source event anywhere in the world
http://moblin-contest.org/redirect.php?banner_id=100url=/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing with a gimbled head.

[tomp]

Dave,

Dave Keeton wrote:
 Thanks Stuart,
   I have been asked to build a machine that can digitize
 complex parts (Landing gear). The catch is that it needs to be a Lights
 Out Operation - fully automated. The only way I can see to do this is
 with a gimbled head and probe on a custom built machine. Thanks for
 looking into it. I think EMC should be able to do this.

   Dave

 On Thu, 2008-11-27 at 22:00 -0600, Stuart Stevenson wrote:
   
 Dave,
As soon as I get the cinci running and comped I will start working
 on the probing.
If you position the gimbaled head and then qualify the probe to a
 standard you will have no issues of accuracy in the gimbaled head. You
 would have access and accuracy.

 On Thu, Nov 27, 2008 at 8:50 AM, Dave Keeton [EMAIL PROTECTED] wrote:
 
 How well does probing and digitizing with a gimbled type spindle work?
 Has any one done this. I would like to use it for digitizing complex
 parts.

Thanks in advance for any ideas offered...
 Dave



 -
 This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
 Build the coolest Linux based applications with Moblin SDK  win great 
 prizes
 Grand prize is a trip for two to an Open Source event anywhere in the world
 http://moblin-contest.org/redirect.php?banner_id=100url=/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users


   
 -
 This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
 Build the coolest Linux based applications with Moblin SDK  win great prizes
 Grand prize is a trip for two to an Open Source event anywhere in the world
 http://moblin-contest.org/redirect.php?banner_id=100url=/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users
 


 -
 This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
 Build the coolest Linux based applications with Moblin SDK  win great prizes
 Grand prize is a trip for two to an Open Source event anywhere in the world
 http://moblin-contest.org/redirect.php?banner_id=100url=/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users

   

thats an interesting project
i have done similar for blades and roots in turbines
the castings vary more than expected

but i always used an 'envelope' to start from ( an 'it oughtta be inside 
this volume' boundary )
( and normals for each probe )
so, speeding up the process was always making the boundary closer to the 
real

but, the reason they needed probing was...
the real surfaces fell outside their original expectations
;)

otherwise every one could just work to 'the numbers'

could you say something about how you approach it?

thanks
tomp


-
This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
Build the coolest Linux based applications with Moblin SDK  win great prizes
Grand prize is a trip for two to an Open Source event anywhere in the world
http://moblin-contest.org/redirect.php?banner_id=100url=/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing (was Re: Homing)

[Stuart Stevenson]

Gentlemen,
   A comment on the probing cycle at the URL in Jeff's post.
   If the center of the probe is not EXACTLY aligned with the
centerline of the spindle the coordinates obtained will not be
accurate to the center of the spindle. A probe calibration routine to
determine and save the inaccuracy on X and Y will need to be done
before any probing. This would need to be incorporated into the probe
cycle at the URL.
thanks
Stuart

-
This SF.Net email is sponsored by the Moblin Your Move Developer's challenge
Build the coolest Linux based applications with Moblin SDK  win great prizes
Grand prize is a trip for two to an Open Source event anywhere in the world
http://moblin-contest.org/redirect.php?banner_id=100url=/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing

[Sam Sokolik]

If you want it really automated - you can set the g10 offsets from the 
probed hole location coordinates.

I have done this for probing tool length (different from what the sample is 
in cvs that sets tool length).  The preview in axis gets a little goofy ;) 
because your cutting path is different than your preview path but it works.

so I don't know if your registering close enough that you could position in 
the hole automatically but either way

-move into hole - either manually or automatically if it is positioned close 
enough
-have the program probe the hole
-calculate center
-set g10 coordinate from calculated center
-run rest of program.

So -




- Original Message - 
From: Chris Radek [EMAIL PROTECTED]
To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net
Sent: Friday, August 31, 2007 2:41 PM
Subject: Re: [Emc-users] probing


 On Fri, Aug 31, 2007 at 01:14:37PM -0500, Stuart Stevenson wrote:
 Gentlemen,
 I have a request. I would like someone to program a probe cycle to
 do this. I would like it in python. I want to have the probing cycle
 for my machine but even more I would like a simple program to compare
 with this to help me learn python.

 Stuart,

 Probing to find the center of a hole can be done strictly inside gcode
 without any external program's help.  The procedure could be:

The operator installs the probe and jogs it into the hole

The operator runs holeprobe.ngc which alternately seeks the X
extents, moves X to the average of them, seeks the Y extents,
moves Y to the average of them, etc.  This will converge very
quickly to the center of the hole and the probe tip size is
irrelevant in the calculation.  (I think this is the algorithm you
proposed or very similar to it.)

With the probe still at the center (but maybe raised),
holeprobe.ngc exits.

Now the operator uses Touch Off to set any coordinate system
however he chooses.

 This seems like a natural and straightforward way to do it.

 That being said, if your intent is to learn python instead, that's
 cool.  But, there are some gotchas that come to mind.  Reading and
 rewriting the var file by an external program while EMC is running is
 likely to cause troubles.  Making a gui for an external python program
 to collect values from the user is a lot of work, and most of what
 you want is already done in AXIS's touch off interface.

 Chris


 -
 This SF.net email is sponsored by: Splunk Inc.
 Still grepping through log files to find problems?  Stop.
 Now Search log events and configuration files using AJAX and a browser.
 Download your FREE copy of Splunk now   http://get.splunk.com/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users 


-
This SF.net email is sponsored by: Splunk Inc.
Still grepping through log files to find problems?  Stop.
Now Search log events and configuration files using AJAX and a browser.
Download your FREE copy of Splunk now   http://get.splunk.com/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing

[Stuart Stevenson]

Gentlemen,
My intention is to have probing cycles. Some will need probe tip
diameter some won't
I want to calibrate the probe to the spindle center.
I want to probe bosses.
I want to probe a square corner. This would probe three time -
twice on one edge and once on a second edge and set the program
rotation and corner point.
I want to set Z with the probe.
I want to probe holes for diameter and adjust offsets automatically.
I want to probe edge locations (distance) and adjust offsets automatically.
I want a gui to allow the operator to choose which probing
operation and the gui will prompt the operator for the information.

I feel I am imposing on someone to turn my request into python. I
certainly couldn't ask someone to implement everything I want as my
wants (needs) can sometimes be pretty extensive.

I want to learn python. I know how I learn. I have to read the
book. Work on the physical portion. Then read the book.

I know it only takes three points to describe a circle and for
most instances this is sufficient. However, I personally know more
than one quality expert who use no less than eight points to inspect a
circle. This is not just for hole center position but they will use
eight points for every hole not matter what they are trying to
determine. Sounds like overkill but they are good and accurate. This
is for just a hole, you ought to see their routine for a cylinder.

thanks
Stuart

-
This SF.net email is sponsored by: Splunk Inc.
Still grepping through log files to find problems?  Stop.
Now Search log events and configuration files using AJAX and a browser.
Download your FREE copy of Splunk now   http://get.splunk.com/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Manfredi Leto]

Hi,

I proposed the problem of manual tool change and offset determination some 
time ago, I have a small mill (always an MF70) without tool holders, so I'm 
very interested.
I'm happy to see there is a first solution for the problem now.

Maybe I will be able to test it in a couple of days.
thanks chris,

Manfredi


My website: www.m24-pro.com
 www.emc2cnc.altervista.org




From: Chris Radek [EMAIL PROTECTED]
Reply-To: Enhanced Machine Controller (EMC) 
emc-users@lists.sourceforge.net
To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] Probing
Date: Sun, 29 Apr 2007 21:18:42 -0500

On Sun, Apr 29, 2007 at 06:52:13PM +0200, Sven Mueller wrote:
  Chris Radek schrieb:
   On Sun, Apr 29, 2007 at 10:03:29AM -0500, Chris Radek wrote:
  
   G49
   insert any tool, touch off, set work coordinate system
   start program
 program probes first tool, THIS is the reference tool for this run
 program saves reference Z coordinate in a variable
 cut...
 program goes up to tool change height, prompts for next tool
 program probes this tool, this - reference = G43
 cut...
 ...
 
  Looks exactly like I would want it to work. It would be nice if this
  could be automated in M06 handling if no tool changer is defined, but
  any working recipe would work for me I guess.


Hi Sven, I've added this scheme to the emc2 cvs trunk.  I can't test
it right now but maybe I can set up something one of these days.

G43 with an H index -1 is now a transient tool whose offsets are
specified on the G43 line.  The length offset is specified with the K
word (and X offset with I word for lathes).

So G43 H-1 K0.5 would do the same thing as G43 H3 if tool 3 has a
length of 0.5 in the tool table.

Like I described above I think this will let you use probing to
measure and set up length compensation for a newly inserted tool in a
fairly straightforward way.

(Since H-1 was previously disallowed, this will not break any
existing programs.)

Chris

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

_
Don't just search. Find. Check out the new MSN Search! 
http://search.msn.com/


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing

[Stuart Stevenson]

Gentlemen,
A lights out machine using probing will have XY registers for each
tool's probing position. This will allow any tool to be probed. They
will usually probe the tool after every tool change to detect broken
tools.
This will also verify the correct tool is in the spindle. An
operator can change a tool in the magazine and put the wrong tool in
the magazine pot. This check is not certain but not many times will
the tool length and XY check position match to the precision necessary
to allow the machine to continue with that tool.
thanks
Stuart

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Sven Mueller]

Chris Radek schrieb:
 Hi Sven, I've added this scheme to the emc2 cvs trunk.  I can't test
 it right now but maybe I can set up something one of these days.

Cool thanks.

It will probably take another week or two until I have a controller for
my machine that EMC2 could work with. And probably another week or two
until I figured out how I need to set up EMC2 to control my machine.

 G43 with an H index -1 is now a transient tool whose offsets are
 specified on the G43 line.  The length offset is specified with the K
 word (and X offset with I word for lathes).
 
 So G43 H-1 K0.5 would do the same thing as G43 H3 if tool 3 has a
 length of 0.5 in the tool table.
 
 Like I described above I think this will let you use probing to
 measure and set up length compensation for a newly inserted tool in a
 fairly straightforward way.
 
 (Since H-1 was previously disallowed, this will not break any
 existing programs.)

Hmm, looks useful, especially if I can call a subroutine upon each tool
change. Speaking of subroutines:

What I would find highly useful would be if emc2 provided
1) Access (readwrite) to the tool lenghts in the tool table
2) Access to the currently selected tool identifier
   (read-only, use T-word to change it)
2) Access (readwrite-once) to the currently set reference tool index.
3) (optional, though ideally available): A way to define that
   subroutine X (a G-Code program) be called on every tool change.

With that, I could define a subroutine which does the following (sorry,
don't know the G-Codes right now, not even wether the conditionals are
available, so I'm using C-like pseudo-code):

idx=cur_ref_tool_idx;
if ( idx==0 ) {
cur_ref_tool_idx=cur_tool;
}
if ( tool_length[cur_tool] == 0 || always_reprobe ) {
execute(G00 Z0);
execute(G00 X probe_pos[X] Y probe_pos[y]);
tmp_length = result_of(probe_length);
if ( check_tool_lengths
  ( tmp_length!=tool_length[cur_tool] ) )
{
abort(Tool length inconsistent for tool $curtool);
}
tool_length[cur_tool]
}
execute(G43 H-1 K tool_length[cur_tool]-tool_length[cur_ref_tool]);
return;

Or in other words: A routing which checks wether a reference tool is
already set. If not, use the current tool index to set it. If the
current tool length is 0 (no previously set), set it to the value
returned from probing at position probe_pos (note: We have a rather
large (regarding our tool sizes), completely even area where the tool
can hit for the probing. Therefor the actual size and shape of the tool
are of minor interest to me regarding this probing.) Finally: set
effective tool length offset to the difference of recorded lengths of
the reference tool and the current tool (which might be the same and the
formula might need a different prefix - i.e. tool_length[cur_ref_tool]
- tool_length[cur_tool]).

Stuart Stevenson wrote about a machine that verifies tool lengths to
mitigate the posibility of broken tools or wrong tools. This would be
achieved with the above subroutine if always_reprobe and
check_tool_lengths are both true. Machines with no tool changers would
set always_reprobe to true and check_tool_length to false. Machines with
tool changers could set both to false and still automatically populate
the tool table with determined tool lengths.

Geeze, would be great if this could be implemented.

Of course, it would be even greater if it was directly available inside
EMC2 with no special requirements in the g-code except for the usual
M06 Tx to select tool x.

BTW: Can I tell EMC2 to automatically go to a specified position on M06
execution so that I could change the tool manually, waiting for
confirmation from me? I might have overlooked it, but I couldn't find
this information in the docs (yet).

regards,
Sven

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Jeff Epler]

On Mon, Apr 30, 2007 at 07:15:33PM +0200, Sven Mueller wrote:
 BTW: Can I tell EMC2 to automatically go to a specified position on M06
 execution so that I could change the tool manually, waiting for
 confirmation from me? I might have overlooked it, but I couldn't find
 this information in the docs (yet).

Yes.  Hidden in the documentation for the AXIS gui is documentation for
the program hal_manualtoolchange.  The hal script
configs/sim/axis_manualtoolchanges shows how to use it.

The tool change position is still programmed as described in the Basic
Configuration section, [EMCIO]TOOL_CHANGE_POSITION.

Jeff

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Sven Mueller]

Chris Radek wrote:
[probe moves]

  It would be nice to be able to set tool length offset this way - but
  currently there is no way to do that, since lengths need to come
  from the tool table.

Hmm, I'm still mostly a newbie regarding EMC. But does the above mean
that EMC can't automatically correct for tool length differences unless
you measure these in advance and store them in the tool table?

Furthermore: If the lengths come from the tool table, what exactly keeps
EMC from feeding the detected tool length differences into the tool
table upon detection?

Regards,
Sven


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 03:34:34PM +0200, Sven Mueller wrote:
 Chris Radek wrote:
 [probe moves]
 
   It would be nice to be able to set tool length offset this way - but
   currently there is no way to do that, since lengths need to come
   from the tool table.
 
 Hmm, I'm still mostly a newbie regarding EMC. But does the above mean
 that EMC can't automatically correct for tool length differences unless
 you measure these in advance and store them in the tool table?

Well yes and no.  In the part of my message you clipped, I mentioned
that you could set a G10 offset using the result of a probe.  But if
you're talking about G43 tool length offset, that's right.

As you can see here,
http://www.linuxcnc.org/handbook/RS274NGC_3/RS274NGC_33a.html#1013768
G43 takes a tool number, not a length - so yes it is intended that
you measure your tools (which are in holders) and put that
information in the tool table.  The G43 length is measured relative
to a reference tool, and you use the reference tool when you set
the coordinate systems, touch off to the work, etc.

Yesterday sat down to change the interpreter so you can specify a
length to G43.  This is a simple change to make but I quickly
found a couple problems/questions:

Currently, G43 H- X- Y- Z- changes the tool offset and then causes
motion to XYZ with the previously set motion type (G0,1,2,3).  I don't
see this behavior described in the ngc spec, but I'm afraid to use
XYZIJK for something else if people use the current behavior.  So
that's problem 1 - I don't know how to allow specification of these
lengths at the gcode level without breaking existing programs.  (If
you guys agree that an existing program that uses this behavior is
NOT ngc, I'd feel less bad about breaking it.)

Even if G43 can take a tool length directly, I couldn't come up with a
straightforward way for the user to use that in gcode.  Imagining the
mill case first because it's simpler: maybe you'd store in a gcode
variable the Z coordinate you get when you probe your reference
tool.  Then when you probe a new tool you'd take the difference and
pass that to G43.  But if someone doesn't have tool holders at all,
I don't know what the reference tool would be, and with no
reference tool I don't know what you'd use to touch-off the work.

Tool length offset is just that - a length - and to measure a length
you need to find the difference between two points.  If you probe a
tool tip, that's only one.  This is problem 2 - I don't quite see a
good way for someone to use G43 in this way, after we solve problem
1.

Chris


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 10:03:29AM -0500, Chris Radek wrote:
 I don't know what the reference tool would be, and with no
 reference tool I don't know what you'd use to touch-off the work.

Replying to myself!  Is it as simple as

G49
insert any tool, touch off, set work coordinate system
start program
  program probes first tool, THIS is the reference tool for this run
  program saves reference Z coordinate in a variable
  cut...
  program goes up to tool change height, prompts for next tool
  program probes this tool, this - reference = G43
  cut...
  ...


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Dave Engvall]

Hi Chris, others.

Really tool length is just part of the problem. A tool number is  
associated with both a tool length and
a tool diameter which may or may not be nominal.
So far I just grit my teeth and work thru the process. I have  
considered (briefly) a procedure to normalize
  the measured lengths against the reference tool and write that
to the tool table.

Dave
On Apr 29, 2007, at 8:03 AM, Chris Radek wrote:

 On Sun, Apr 29, 2007 at 03:34:34PM +0200, Sven Mueller wrote:
 Chris Radek wrote:
 [probe moves]

 It would be nice to be able to set tool length offset this way -  
 but
 currently there is no way to do that, since lengths need to come
 from the tool table.

 Hmm, I'm still mostly a newbie regarding EMC. But does the above mean
 that EMC can't automatically correct for tool length differences  
 unless
 you measure these in advance and store them in the tool table?

 Well yes and no.  In the part of my message you clipped, I mentioned
 that you could set a G10 offset using the result of a probe.  But if
 you're talking about G43 tool length offset, that's right.

 As you can see here,
 http://www.linuxcnc.org/handbook/RS274NGC_3/RS274NGC_33a.html#1013768
 G43 takes a tool number, not a length - so yes it is intended that
 you measure your tools (which are in holders) and put that
 information in the tool table.  The G43 length is measured relative
 to a reference tool, and you use the reference tool when you set
 the coordinate systems, touch off to the work, etc.

 Yesterday sat down to change the interpreter so you can specify a
 length to G43.  This is a simple change to make but I quickly
 found a couple problems/questions:

 Currently, G43 H- X- Y- Z- changes the tool offset and then causes
 motion to XYZ with the previously set motion type (G0,1,2,3).  I don't
 see this behavior described in the ngc spec, but I'm afraid to use
 XYZIJK for something else if people use the current behavior.  So
 that's problem 1 - I don't know how to allow specification of these
 lengths at the gcode level without breaking existing programs.  (If
 you guys agree that an existing program that uses this behavior is
 NOT ngc, I'd feel less bad about breaking it.)

 Even if G43 can take a tool length directly, I couldn't come up with a
 straightforward way for the user to use that in gcode.  Imagining the
 mill case first because it's simpler: maybe you'd store in a gcode
 variable the Z coordinate you get when you probe your reference
 tool.  Then when you probe a new tool you'd take the difference and
 pass that to G43.  But if someone doesn't have tool holders at all,
 I don't know what the reference tool would be, and with no
 reference tool I don't know what you'd use to touch-off the work.

 Tool length offset is just that - a length - and to measure a length
 you need to find the difference between two points.  If you probe a
 tool tip, that's only one.  This is problem 2 - I don't quite see a
 good way for someone to use G43 in this way, after we solve problem
 1.

 Chris


 -- 
 ---
 This SF.net email is sponsored by DB2 Express
 Download DB2 Express C - the FREE version of DB2 express and take
 control of your XML. No limits. Just data. Click to get it now.
 http://sourceforge.net/powerbar/db2/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 08:27:00AM -0700, Dave Engvall wrote:
 Hi Chris, others.
 
 Really tool length is just part of the problem. A tool number is  
 associated with both a tool length and
 a tool diameter which may or may not be nominal.
 So far I just grit my teeth and work thru the process. I have  
 considered (briefly) a procedure to normalize
   the measured lengths against the reference tool and write that
 to the tool table.
 
 Dave

Dave, I think you and I have tool holders with tools in them pretty
much permanently, and I agree it's a complex matter to measure them
well, but no matter how we get it done, we can end up with the right
data in the tool table and the current scheme in emc can work for us.

There is another setup where the user has something like a dremel
tool collet or jacobs chuck and a bunch of loose tools.  I used to
have this, and emc doesn't work very well with it.  For this setup,
using lengths from the tool table is useless.  For radius, it's
still possible to use the tool table though.  

For lengths, the user really wants to be able to stick in the tool
and tighten it down, and have emc measure it and cut at the right
height.  I think we can do this pretty well with the probing, it's
just a matter of details.

Chris


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Dave Engvall]

Hi Chris,

You are quite correct in assuming I have a series of tool holders;  
however I do a lot of one-off stuff
in which the tooling outruns the number of tool holders I have.
With the right probe and program we ought to be able to gage  both  
length and diameter
in a manner analogous to the laser setups that measure both length  
and diameter. Gaging
the diameter is going to be the most difficult.
After that as someone on this list once said: it is simply a matter  
of software.

Dave
On Apr 29, 2007, at 8:35 AM, Chris Radek wrote:

 On Sun, Apr 29, 2007 at 08:27:00AM -0700, Dave Engvall wrote:
 Hi Chris, others.

 Really tool length is just part of the problem. A tool number is
 associated with both a tool length and
 a tool diameter which may or may not be nominal.
 So far I just grit my teeth and work thru the process. I have
 considered (briefly) a procedure to normalize
   the measured lengths against the reference tool and write that
 to the tool table.

 Dave

 Dave, I think you and I have tool holders with tools in them pretty
 much permanently, and I agree it's a complex matter to measure them
 well, but no matter how we get it done, we can end up with the right
 data in the tool table and the current scheme in emc can work for us.

 There is another setup where the user has something like a dremel
 tool collet or jacobs chuck and a bunch of loose tools.  I used to
 have this, and emc doesn't work very well with it.  For this setup,
 using lengths from the tool table is useless.  For radius, it's
 still possible to use the tool table though.

 For lengths, the user really wants to be able to stick in the tool
 and tighten it down, and have emc measure it and cut at the right
 height.  I think we can do this pretty well with the probing, it's
 just a matter of details.

 Chris


 -- 
 ---
 This SF.net email is sponsored by DB2 Express
 Download DB2 Express C - the FREE version of DB2 express and take
 control of your XML. No limits. Just data. Click to get it now.
 http://sourceforge.net/powerbar/db2/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 https://lists.sourceforge.net/lists/listinfo/emc-users


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Dave Engvall]

Hi Chris,

After thinking about it a bit. Are you proposing a tool  referenced  
against the zero tool
after every (manual) tool change? That would take time but would work  
for non-tool holder machines
i.e. collet on the spindle as well as those of us with tool holders.
Might make a really nice option.

Dave
On Apr 29, 2007, at 8:44 AM, Dave Engvall wrote:

 Hi Chris,

 You are quite correct in assuming I have a series of tool holders;
 however I do a lot of one-off stuff
 in which the tooling outruns the number of tool holders I have.
 With the right probe and program we ought to be able to gage  both
 length and diameter
 in a manner analogous to the laser setups that measure both length
 and diameter. Gaging
 the diameter is going to be the most difficult.
 After that as someone on this list once said: it is simply a matter
 of software.

 Dave
 On Apr 29, 2007, at 8:35 AM, Chris Radek wrote:

 On Sun, Apr 29, 2007 at 08:27:00AM -0700, Dave Engvall wrote:
 Hi Chris, others.

 Really tool length is just part of the problem. A tool number is
 associated with both a tool length and
 a tool diameter which may or may not be nominal.
 So far I just grit my teeth and work thru the process. I have
 considered (briefly) a procedure to normalize
   the measured lengths against the reference tool and write that
 to the tool table.

 Dave


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 08:57:22AM -0700, Dave Engvall wrote:
 Hi Chris,
 
 After thinking about it a bit. Are you proposing a tool  referenced  
 against the zero tool
 after every (manual) tool change? That would take time but would work  
 for non-tool holder machines
 i.e. collet on the spindle as well as those of us with tool holders.
 Might make a really nice option.
 
 Dave

Yes that's what I propose would be possible if we allow G43 length
specifiation directly in gcode as well as from the tool table.


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Sven Mueller]

Chris Radek wrote:

 Even if G43 can take a tool length directly, I couldn't come up with a
 straightforward way for the user to use that in gcode.  Imagining the
 mill case first because it's simpler: maybe you'd store in a gcode
 variable the Z coordinate you get when you probe your reference
 tool.  Then when you probe a new tool you'd take the difference and
 pass that to G43.  But if someone doesn't have tool holders at all,
 I don't know what the reference tool would be, and with no
 reference tool I don't know what you'd use to touch-off the work.
 
 Tool length offset is just that - a length - and to measure a length
 you need to find the difference between two points.  If you probe a
 tool tip, that's only one.  This is problem 2 - I don't quite see a
 good way for someone to use G43 in this way, after we solve problem
 1.

Hmm, I have a small hobby-grade CNC machine (a modified Proxxon MF70
from usovo.de) which doesn't have a tool holder. It came with PC/NC, a
DOS program. This program takes the following approach for tool length
corrections:

It basically assumes that the first tool you use is the one you used to
define your coordinate system. (PC/NC allows redefining X/Y/Z origins
per g-code file, though this is a non-gcode manual process, which also
involves options to define the working space, with an error issued when
you g-code exceeds this working space. It also allows defining
independent scaling for the X and Y axes, not sure about Z at the
moment.) All origin, offset and working area settings are done before
the first line of G-Code is executed.

Anyway, the process in PC/NC works like this:
Define working area in X, Y dimensions (machine coordinates), define
origin in X, Y and Z (machine coordinates) for G-Code. This all usually
happens with the first tool you intend to use.
You need to measure the tool length before setting X/Y/Z origins and
that tool length (or rather: The Z coordinate at whicht the tool hit the
measurement switch) is used as a reference.
Whenever PC/NC reaches another M06 T?, it will _always_ measure the
tool anew, even if it has a known length for that tool number. It then
uses the difference in Z to correct the tool length.

I would hope that EMC at one time also provides a similar functionality.
Especially as manual tool changes are prone to errors with the depth to
which a tool is inserted into the spindle.

However, PC/NC also has problems with tool changes. Imagine the
following G-Code:

M06 T02
G01 X1 Y1 Z0
M06 T03
G01 X1 Y1 Z0

Looks pretty simple, doesn't it? Now, what happens in PC/NC?
0) (store current position)
1) move to tool change position
2) ask for tool to be changed (which you confirm)
3) move to stored position
4) move to maximum Z on measurement X/Y
5) measure tool
6) move to stored position
7) execute G01 X1 Y1 Z0 (and store that position)
8) move to tool change position
9) ask for tool change (which you confirm)
10) move to stored position
(without correction, since it is not yet measured)
11) move to maximum Z on measurement X/Y
12) measure tool
13) move to stored position (with corrected tool length)
14) execute G01 X1 Y1 Z0 (with corrected tool length)

Now imagine what happens it T03 is longer than T02. Right, it either
breaks or damages the stock when (10) is done.

Regards,
Sven

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Sven Mueller]

Chris Radek schrieb:
 On Sun, Apr 29, 2007 at 10:03:29AM -0500, Chris Radek wrote:
 I don't know what the reference tool would be, and with no
 reference tool I don't know what you'd use to touch-off the work.
 
 Replying to myself!  Is it as simple as
 
 G49
 insert any tool, touch off, set work coordinate system
 start program
   program probes first tool, THIS is the reference tool for this run
   program saves reference Z coordinate in a variable
   cut...
   program goes up to tool change height, prompts for next tool
   program probes this tool, this - reference = G43
   cut...
   ...

Looks exactly like I would want it to work. It would be nice if this
could be automated in M06 handling if no tool changer is defined, but
any working recipe would work for me I guess.

Regards,
Sven

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Sven Mueller]

Dave Engvall schrieb:
 Really tool length is just part of the problem. A tool number is  
 associated with both a tool length and
 a tool diameter which may or may not be nominal.

Right, but a tools diameter doesn't change, no matter what you do while
you insert it. However, it's felt length might change if you don't
insert it to the same depth each time.

Though I could imagine a machine setup where even the tool diameter
could be measured: Just first measure the length, then move the tip
horizontally against a second switch. If you already measured another
tool, you can take the horizontal difference between the two moves to
detect the tools radius relative to the first tool.

Regards,
Sven

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Ray Henry]

I guess I don't really see the issue here with tool length and diameter
probing.  Years ago now I wrote a little tickle script that allowed me
to turn the probe switch over, pressed it with the tool and from the
known height of that switch, wrote those values to the tool table and
then reread the table.  This could easily be done again from any of the
guis.  Tickle's automated menu would allow a user to add just the tool
probe code to a directory and it would be useable from tkemc or mini.

As for setting work offsets, that is easy enough now.

You'll be hard pressed to find the correct xy location for a tool length
measure because it really depends upon the tool being used. Imagine a
drill vs a face mill or fly cutter and you should be able to see that a
single xy location will not probe them both properly.  

Manual tool probing is really easy and is the way most of the commercial
machines work anyway.  I suppose there are some lights out shops that
have a tool hive that replaces dull tools where the new ones require an
automated tool measure but that is quite a way from where EMC is now.

HTH

Rayh


On Sun, 2007-04-29 at 18:49 +0200, Sven Mueller wrote:
 Chris Radek wrote:
 
  Even if G43 can take a tool length directly, I couldn't come up with a
  straightforward way for the user to use that in gcode.  Imagining the
  mill case first because it's simpler: maybe you'd store in a gcode
  variable the Z coordinate you get when you probe your reference
  tool.  Then when you probe a new tool you'd take the difference and
  pass that to G43.  But if someone doesn't have tool holders at all,
  I don't know what the reference tool would be, and with no
  reference tool I don't know what you'd use to touch-off the work.
  
  Tool length offset is just that - a length - and to measure a length
  you need to find the difference between two points.  If you probe a
  tool tip, that's only one.  This is problem 2 - I don't quite see a
  good way for someone to use G43 in this way, after we solve problem
  1.
 
 Hmm, I have a small hobby-grade CNC machine (a modified Proxxon MF70
 from usovo.de) which doesn't have a tool holder. It came with PC/NC, a
 DOS program. This program takes the following approach for tool length
 corrections:
 
 It basically assumes that the first tool you use is the one you used to
 define your coordinate system. (PC/NC allows redefining X/Y/Z origins
 per g-code file, though this is a non-gcode manual process, which also
 involves options to define the working space, with an error issued when
 you g-code exceeds this working space. It also allows defining
 independent scaling for the X and Y axes, not sure about Z at the
 moment.) All origin, offset and working area settings are done before
 the first line of G-Code is executed.
 
 Anyway, the process in PC/NC works like this:
 Define working area in X, Y dimensions (machine coordinates), define
 origin in X, Y and Z (machine coordinates) for G-Code. This all usually
 happens with the first tool you intend to use.
 You need to measure the tool length before setting X/Y/Z origins and
 that tool length (or rather: The Z coordinate at whicht the tool hit the
 measurement switch) is used as a reference.
 Whenever PC/NC reaches another M06 T?, it will _always_ measure the
 tool anew, even if it has a known length for that tool number. It then
 uses the difference in Z to correct the tool length.
 
 I would hope that EMC at one time also provides a similar functionality.
 Especially as manual tool changes are prone to errors with the depth to
 which a tool is inserted into the spindle.
 
 However, PC/NC also has problems with tool changes. Imagine the
 following G-Code:
 
 M06 T02
 G01 X1 Y1 Z0
 M06 T03
 G01 X1 Y1 Z0
 
 Looks pretty simple, doesn't it? Now, what happens in PC/NC?
 0) (store current position)
 1) move to tool change position
 2) ask for tool to be changed (which you confirm)
 3) move to stored position
 4) move to maximum Z on measurement X/Y
 5) measure tool
 6) move to stored position
 7) execute G01 X1 Y1 Z0 (and store that position)
 8) move to tool change position
 9) ask for tool change (which you confirm)
 10) move to stored position
 (without correction, since it is not yet measured)
 11) move to maximum Z on measurement X/Y
 12) measure tool
 13) move to stored position (with corrected tool length)
 14) execute G01 X1 Y1 Z0 (with corrected tool length)
 
 Now imagine what happens it T03 is longer than T02. Right, it either
 breaks or damages the stock when (10) is done.
 
 Regards,
 Sven
 
 -
 This SF.net email is sponsored by DB2 Express
 Download DB2 Express C - the FREE version of DB2 express and take
 control of your XML. No limits. Just data. Click to get it now.
 http://sourceforge.net/powerbar/db2/
 ___
 Emc-users mailing list
 Emc-users@lists.sourceforge.net
 

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 12:04:25PM -0500, Ray Henry wrote:
 
 I guess I don't really see the issue here with tool length and diameter
 probing.  Years ago now I wrote a little tickle script that allowed me
 to turn the probe switch over, pressed it with the tool and from the
 known height of that switch, wrote those values to the tool table and
 then reread the table.  This could easily be done again from any of the
 guis.  Tickle's automated menu would allow a user to add just the tool
 probe code to a directory and it would be useable from tkemc or mini.

This sounds like a good way to configure a tool table if you have
holders, but is not useful for changing tools (a different depth 
every time you insert them) during a program run.

 You'll be hard pressed to find the correct xy location for a tool length
 measure because it really depends upon the tool being used. Imagine a
 drill vs a face mill or fly cutter and you should be able to see that a
 single xy location will not probe them both properly.  

True enough.  This wouldn't be useful for a machine using tools like
that.  With end mills and drill bits, though, it would be fine.  On
my small machine I don't think I've ever cut with anything but end
mills, engraving cutters, and drill bits.  They can all be measured
at the same point.


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing

[Stuart Stevenson]

Gentlemen,
Tool length offsetting is BIG subject. It is difficult to get
people to agree on what it is and where it should be measured from.
You must determine how you are going to do it in your shop and then be
consistent with it.
I have two machines that need the tool lengths set to the
programmed tool length. These are 5 axis machines with controls that
do not have 5 axis tool length compensation. I have a tool setting
station to determine and set the tool lengths.
I have two 5 axis machines that have 5 axis tool length compensation.
I can set a tool length in my tool setter and use it in any
machine. We have determined the tool set gauge point for every machine
and adjusted the parameters.
I said all that to make this point. The most flexible way is the
best. My machines with the newest controls have tool change
subroutines that are called by the main gcode program. This allows
calculations and comparisons and the writing of tool attributes to the
tool table(file).
All gcode programs program the center of the spindle and the pivot
point of any rotary axis the spindle moves on. The tool length
compensation adjusts this to the machine and each particular setup.
Three axis machines and multiaxis machines in which the tool axis
spindle does not rotate are much simpler to set the tool length. You
can set the tool length as a minus number from the z axis home
position to the tool set zero position or the program zero position.
A machine that tilts the spindle will have a different tool offset
requirement. To use a 4 or 5 axis tool length offset you will need to
use positive numbers in the tool length table. This tool length value
and the pivot length value in the control will have to sum to the
length from the pivot point to the tool tip. When the tools lengths
are set in this manner you will be able to use the same tools and tool
lengths in a 3 axis or 4 axis or 5 axis program.
There is on gotcha in this. You WILL have to deal with it. When
the tool length offset is cancelled the machine will try to move the
gauge point down to the programmed Z point.
I have a couple machines that will offset the machine as soon as
the offset is changed. These machines respond in the same manner for
g54 work center offsets and tool length offset. I don't like this type
of response. I much prefer the machine to read offset register and
adjust during the next commanded move.
   BTW, does EMC have 5 axis tool length offsets? Does EMC have 5 axis
tool radius compensation?
thanks
Stuart

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] probing

[Chris Radek]

On Sun, Apr 29, 2007 at 12:17:56PM -0500, Stuart Stevenson wrote:
 I have a couple machines that will offset the machine as soon as
 the offset is changed. These machines respond in the same manner for
 g54 work center offsets and tool length offset. I don't like this type
 of response. I much prefer the machine to read offset register and
 adjust during the next commanded move.

EMC doesn't move when you change the tool length offset.  It adjusts
the end of the following move.

BTW, does EMC have 5 axis tool length offsets? Does EMC have 5 axis
 tool radius compensation?

No, no.


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sun, Apr 29, 2007 at 06:52:13PM +0200, Sven Mueller wrote:
 Chris Radek schrieb:
  On Sun, Apr 29, 2007 at 10:03:29AM -0500, Chris Radek wrote:
  
  G49
  insert any tool, touch off, set work coordinate system
  start program
program probes first tool, THIS is the reference tool for this run
program saves reference Z coordinate in a variable
cut...
program goes up to tool change height, prompts for next tool
program probes this tool, this - reference = G43
cut...
...
 
 Looks exactly like I would want it to work. It would be nice if this
 could be automated in M06 handling if no tool changer is defined, but
 any working recipe would work for me I guess.


Hi Sven, I've added this scheme to the emc2 cvs trunk.  I can't test
it right now but maybe I can set up something one of these days.

G43 with an H index -1 is now a transient tool whose offsets are
specified on the G43 line.  The length offset is specified with the K
word (and X offset with I word for lathes).

So G43 H-1 K0.5 would do the same thing as G43 H3 if tool 3 has a
length of 0.5 in the tool table.

Like I described above I think this will let you use probing to
measure and set up length compensation for a newly inserted tool in a
fairly straightforward way.

(Since H-1 was previously disallowed, this will not break any
existing programs.)

Chris

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[John Kasunich]

Eric H. Johnson wrote:
 Hi all,
 
 In reading about the probe function it looks to do something close to what I
 would like to do with a touch plate. This touch plate is put on top of the
 material and Z is lowered until the tool touches the plate, which completes
 the circuit and turns on an input. 
 
 When this occurs, I would like to do the equivalent of a G92 Z0.375 (the
 pad is 3/8) or some other means of establishing this point as the top of
 the material. Is there a way to use the probe function, or any other means
 of performing this?
 
 Regards,
 Eric
 
It sounds like you are trying to home to the touch plate...

In that case, what if you wired the touch plate up as a home switch for 
the Z axis?

Or do you already have a real home switch, and simply want to establish
an offset coordinate system using the touch plate?

Regards,

John Kasunich

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Eric H. Johnson]

John, 

Yes, I already have a home, and I am trying to do exactly as you say,
establish an offset coordinate system using the touch plate.

Regards,
Eric

 It sounds like you are trying to home to the touch plate...
 
 In that case, what if you wired the touch plate up as a home 
 switch for the Z axis?
 
 Or do you already have a real home switch, and simply want to 
 establish an offset coordinate system using the touch plate?


-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Probing

[Chris Radek]

On Sat, Apr 28, 2007 at 05:21:25PM -0400, John Kasunich wrote:
 
 I believe you can do a probe and have it print (or write to a file) the
 probed position, then do a G92 whatever...  I don't know of a way to
 combine those steps into a single operation.  High level stuff like
 g-code isn't my strong area though.
 
 Regards,
 
 John Kasunich

A probe move records the trigger coordinates in gcode variables.  It
should be a simple matter to use G10 L2 ... to set an offset using the
result.

It would be nice to be able to set tool length offset this way - but
currently there is no way to do that, since lengths need to come
from the tool table.

Chris

-
This SF.net email is sponsored by DB2 Express
Download DB2 Express C - the FREE version of DB2 express and take
control of your XML. No limits. Just data. Click to get it now.
http://sourceforge.net/powerbar/db2/
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users