Re: [Emc-users] Cutter compensation

[Stuart Stevenson]

In aerospace shops there is usually a requirement for certification of the
NCcode that produces the part. This means gcode that is in the CNC machine
must come from a secure directory on your system. To be written in the
secure directory the program must be certified by inspection the parts
created by the program meet all the criteria on the work order referencing
the purchase order. All programs in the secure directory are read only and
can only be written into the directory by specific personnel. Going to your
CAM system to reprocess a program to change a tool will then trigger
another First Part Inspection to recertify the NCcode. The whole exercise
must be documented in the quality system subject to audit at a future time.
This is a MAJOR PITA and a very costly event. Changing the gcode program is
not very useful in this environment. Cutter compensation is very useful.
Multiple tools of every finishing size is also very useful and will not
trigger recertification of the program.
Boeing calls this DPD (Digital Product Definition). I don't know if it is
still referred to as this but I am certain the requirements are still in
place no matter what it is called. Every aerospace OEM will have a similar
expectation and will audit to monitor compliance.

It gets to the point some OEMs require any change in the shop plan (router)
requires submission to the OEM for recertification of the shop plan.


On Tue, Sep 8, 2020 at 11:19 AM N  wrote:

> > On 09/07/2020 03:24 PM, Leonardo Marsaglia wrote:
> > > Is it any advantage in using cutter compensation when programming the
> > > g-code using CAM? Because since I've started working with CAM for my
> > > turning programs I like to let the software do all the compensation.
> By the
> > > way, I'm talking only about lathe programs. I don't know if this could
> be
> > > an advantage for the mill machine user.
> > >
> > >
> > The advantage is you can adjust the size of the part or
> > compensate for tool wear without recreating the G-code.
> > This is less of an issue today than when G-code programs
> > came on punched paper tapes.
>
> For me it still sound like a very good idea fine tuning diameter instead
> of changing the g-code.
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>


-- 
Addressee is the intended audience.
If you are not the addressee then my consent is not given for you to read
this email furthermore it is my wish you would close this without saving or
reading, and cease and desist from saving or opening my private
correspondence.
Thank you for honoring my wish.

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

Re: [Emc-users] Cutter compensation

[N]

> On 09/07/2020 03:24 PM, Leonardo Marsaglia wrote:
> > Is it any advantage in using cutter compensation when programming the
> > g-code using CAM? Because since I've started working with CAM for my
> > turning programs I like to let the software do all the compensation. By the
> > way, I'm talking only about lathe programs. I don't know if this could be
> > an advantage for the mill machine user.
> >
> >
> The advantage is you can adjust the size of the part or 
> compensate for tool wear without recreating the G-code.  
> This is less of an issue today than when G-code programs 
> came on punched paper tapes.

For me it still sound like a very good idea fine tuning diameter instead of 
changing the g-code.


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

Re: [Emc-users] Cutter compensation

[andy pugh]

On Tue, 8 Sep 2020 at 01:17, Leonardo Marsaglia  wrote:
>
> . I only have to compensate for Z and
> X differences when they are too much of a trouble for the finishing
> grinding process after, and I usually do that by hand  from time to time. I
> certainly can give cutter compensation a try.

Manual G43.2 might be a good way to do that.

-- 
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] Cutter compensation

[Leonardo Marsaglia]

Thanks for the feedback guys. I'm too used to not using tool wear
compensation that I forget about that. I only have to compensate for Z and
X differences when they are too much of a trouble for the finishing
grinding process after, and I usually do that by hand  from time to time. I
certainly can give cutter compensation a try.

El lun., 7 sept. 2020 a las 20:49, Jon Elson ()
escribió:

> On 09/07/2020 03:24 PM, Leonardo Marsaglia wrote:
> > Is it any advantage in using cutter compensation when programming the
> > g-code using CAM? Because since I've started working with CAM for my
> > turning programs I like to let the software do all the compensation. By
> the
> > way, I'm talking only about lathe programs. I don't know if this could be
> > an advantage for the mill machine user.
> >
> >
> The advantage is you can adjust the size of the part or
> compensate for tool wear without recreating the G-code.
> This is less of an issue today than when G-code programs
> came on punched paper tapes.
>
> Jon
>
>
> ___
> 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] Cutter compensation

[Jon Elson]

On 09/07/2020 03:24 PM, Leonardo Marsaglia wrote:

Is it any advantage in using cutter compensation when programming the
g-code using CAM? Because since I've started working with CAM for my
turning programs I like to let the software do all the compensation. By the
way, I'm talking only about lathe programs. I don't know if this could be
an advantage for the mill machine user.


The advantage is you can adjust the size of the part or 
compensate for tool wear without recreating the G-code.  
This is less of an issue today than when G-code programs 
came on punched paper tapes.


Jon


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

Re: [Emc-users] Cutter compensation

[N]

Could change cutter diameter and program still works but this should be the 
only advantage.

Used CAM module, "path workbench" in Freecad, not sure if I made some error but 
it did not work well for me. Simple path, should have an arc in each corner. It 
upper right corner it decided some kind of pecking cycle was a good idea, 
drilling an arc of tightly space holes. Source is available so it should be 
possibe to do something about it and think the back is good.

> Is it any advantage in using cutter compensation when programming the
> g-code using CAM? Because since I've started working with CAM for my
> turning programs I like to let the software do all the compensation. By the
> way, I'm talking only about lathe programs. I don't know if this could be
> an advantage for the mill machine user.
> 
> El lun., 7 sept. 2020 a las 16:51, N ()
> escribió:
> 
> > > On Mon, 7 Sep 2020 at 20:20, N  wrote:
> > > >
> > > > First thing I noticed then reading about cutter compensation is some
> > use G41,G42 while Linuxcnc use G42,G43 for different side of cutter.
> > >
> > > I don't think so. G43 is cutter _length_ compensation.
> >
> > Yes reading again, work to long days and are probably to tired, don't know
> > why I mixed them up. Though still got some confusing movements.


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

Re: [Emc-users] Cutter compensation

[Ed]

On 9/7/20 2:48 PM, N wrote:

On Mon, 7 Sep 2020 at 20:20, N  wrote:

First thing I noticed then reading about cutter compensation is some use 
G41,G42 while Linuxcnc use G42,G43 for different side of cutter.

I don't think so. G43 is cutter _length_ compensation.

Yes reading again, work to long days and are probably to tired, don't know why 
I mixed them up. Though still got some confusing movements.


Make your last Z move above Z0 or have the cutter well clear before you 
cancel cutter comp. The next move after cancelling will move the 
effective cutting line back to the center of the cutter, if it is near 
to a surface it may clip it on the way.



Ed.




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

Re: [Emc-users] Cutter compensation

[Leonardo Marsaglia]

Is it any advantage in using cutter compensation when programming the
g-code using CAM? Because since I've started working with CAM for my
turning programs I like to let the software do all the compensation. By the
way, I'm talking only about lathe programs. I don't know if this could be
an advantage for the mill machine user.

El lun., 7 sept. 2020 a las 16:51, N ()
escribió:

> > On Mon, 7 Sep 2020 at 20:20, N  wrote:
> > >
> > > First thing I noticed then reading about cutter compensation is some
> use G41,G42 while Linuxcnc use G42,G43 for different side of cutter.
> >
> > I don't think so. G43 is cutter _length_ compensation.
>
> Yes reading again, work to long days and are probably to tired, don't know
> why I mixed them up. Though still got some confusing movements.
>
>
> ___
> 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] Cutter compensation

[N]

> On Mon, 7 Sep 2020 at 20:20, N  wrote:
> >
> > First thing I noticed then reading about cutter compensation is some use 
> > G41,G42 while Linuxcnc use G42,G43 for different side of cutter.
> 
> I don't think so. G43 is cutter _length_ compensation.

Yes reading again, work to long days and are probably to tired, don't know why 
I mixed them up. Though still got some confusing movements.


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

Re: [Emc-users] Cutter compensation

[andy pugh]

On Mon, 7 Sep 2020 at 20:20, N  wrote:
>
> First thing I noticed then reading about cutter compensation is some use 
> G41,G42 while Linuxcnc use G42,G43 for different side of cutter.

I don't think so. G43 is cutter _length_ compensation.

http://linuxcnc.org/docs/2.8/html/gcode.html

-- 
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] Cutter compensation

[N]

First thing I noticed then reading about cutter compensation is some use 
G41,G42 while Linuxcnc use G42,G43 for different side of cutter.

Sometimes I get a little bit confusing moves. Turning off cutter compensation 
with G40 and move in one direction only and it seems to decompensate in other 
direction. Happen to know if these are well defined for all cases? Or if there 
are any issues?


Regards Nicklas Karlsson


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

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Tuesday 07 August 2018 04:10:25 andy pugh wrote:

> On 7 August 2018 at 01:00, Gene Heskett  wrote:
> > I was thinking in terms of carving the example/lathe pawn. None of
> > the shown positions can carve it exactly
>
Without gouging.

> I think you are confusing positions and angles still.
> I am pretty sure that position 2 with an MVJNR holder (VNMG tip) can
> do it Front angle of 87, back angle of 52.

That is also likely true, if those angles are set in the tool.tbl. TBT 
the lack of a known orientation for 0.00 degrees (until this thread) and 
the weird results I got by looking up the chip and putting that raw data 
into the tool.tbl, (and I don't believe I have any VNMG chips as I 
usually order the wider diamond shape) and the wasted material that gave 
me, has since precluded my doing so, simply because what I was doing was 
wrong in light of 0.00 being along the Z axis. I don't have an instant 
project to test how that works, but I will try it next time I do.

It would be a great help to me, if the boxes these chips came in had not 
only the makers part number, but also the "VNMG/whatever" that specifies 
the shape, size and the tip radii, and side angles printed right on the 
box. But having that info right on the box w/o have to go to the makers 
web site be be enlightened, thats pretty rare if not entirely missing.

Point being that this stuff can run north of $200 for a box of 10, so how 
much more would it cost to print a proper label? Not having it is bs, 
and wastes a persons time trying to find it online. And this is turning 
into a rant on my part, sorry.

> http://www.aydosa-tools.com/index.php/mvjnr-l-93-external-top-clamp-tu
>rning-toolholder



-- 
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)
Genes Web page 

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[andy pugh]

On 7 August 2018 at 01:00, Gene Heskett  wrote:

> I was thinking in terms of carving the example/lathe pawn. None of the
> shown positions can carve it exactly

I think you are confusing positions and angles still.
I am pretty sure that position 2 with an MVJNR holder (VNMG tip) can do it
Front angle of 87, back angle of 52.
http://www.aydosa-tools.com/index.php/mvjnr-l-93-external-top-clamp-turning-toolholder

-- 
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, 1916

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Monday 06 August 2018 05:18:31 andy pugh wrote:

> On 6 August 2018 at 03:36, Gene Heskett  wrote:
> > Tool paths (corrected) are I assume to be the nearest of the 8
> > positions, or are those actually calculated from data in the tool
> > table (and fussed about if obviously wrong I hope.
>
> Tool radius correction is based entirely on the stated tool
> orientation in the tool table.
> It take no account of the stated front and back angles.
> If you want an orientation 2 tool with the cutter flanks pointing back
> in to the work then Axis will cheerfully render that for you while at
> the same time the motion planner will do radius compensation for an
> orientation 2 tool.
>
> The tool controlled point can only be at 9 positions relative to the
> centre point of the tool tip radius. This has very little to do with
> the flank angles. It is more related to which quadrants of a notional
> full-circle tool are in use.
> For example orienation 2 (right hand facing and turning) expects to be
> touching at 12-o-clock when moving purely in Z and at 9-o-clock when
> facing in X. If moving in some combination then the tool will be moved
> a little bit closer to the work to compensate for the gap between the
> controlled point and the tool tip that exists between those two
> tangents.
>
> For the vast majority of lathe work cutter comp is not important. The
> positions of  shoulders and absolute diameters are unaffected. Tapers
> will end up a little fatter than drawn and both external and internal
> fillets will have extra material. The latter vary rarely matters, and
> the former normally seem to need some tweaking-to-fit anyway, so I run
> with cutter-comp turned off nearly all the time.
> If I was machining accurate spheres then things would be different.

I was thinking in terms of carving the example/lathe pawn. None of the 
shown positions can carve it exactly, the best you can do it to steer it 
ccw enough that the side of the chip clears for all motions, and ignore 
the cutter comp.

And I have discovered there are two versions of that pawn in the wild, 
the 2nd one looks to have been generated by a cad proggy but it does 
know about looping better than the original. It would take a bit longer  
but with its thinner cuts, the spindle revs could be setup as CCS mode, 
gaining back some of the lost time.  Both make good practice at cutting 
air, but I've never actually made one. :)


-- 
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)
Genes Web page 

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Ken Strauss]

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, August 05, 2018 11:06 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] Cutter compensation with mill turning
>
> On Sunday 05 August 2018 22:39:18 Ken Strauss wrote:
>
> > > -Original Message-
> > > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > > Sent: Sunday, August 05, 2018 10:27 PM
> > > To: emc-users@lists.sourceforge.net
> > > Subject: Re: [Emc-users] Cutter compensation with mill turning

> Particularly if you raise the motor power, the TTS may slip in its holder
> as it has no provision to keylock it to the spindle. It seriously needs
> a keying slot cut into the side, and a locking pin to engage that slot
> in the spindle. When I went of a spree and cut up 12 feet of 7/8" brass
> for tap holders, I skipped the TTS and cut a semi-circle to fit the head
> of a 4mm socket head cap screw into the edge of a 7/8" r8 so the tap is
> keyed into the r8, which is keyed into my spindle. zero tap  slippage
> now. An er20 takes 18" wrenches tightened seriously to get a good enough
> grip on a 4mm.7 tap. With my psu and a Pico pwm-servo amp, I'm getting
> close to 2hp out of the factory G0704 motor.  Its almost enough to turn
> a 12mm tap in steel.  And will get the job done if I "peck" it.  How
> long those plastic backgears would last doing that is Yet To Be
> Determined. :)
> >

Yes, TTS will pullout particularly with heavy cutting coupled with chatter.
Tormach has recognized the problem and offers a NMTB30 spindle on their
recently announced PCNC1100MX.



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[andy pugh]

On 6 August 2018 at 03:36, Gene Heskett  wrote:

> Tool paths (corrected) are I assume to be the nearest of the 8 positions,
> or are those actually calculated from data in the tool table (and fussed
> about if obviously wrong I hope.

Tool radius correction is based entirely on the stated tool
orientation in the tool table.
It take no account of the stated front and back angles.
If you want an orientation 2 tool with the cutter flanks pointing back
in to the work then Axis will cheerfully render that for you while at
the same time the motion planner will do radius compensation for an
orientation 2 tool.

The tool controlled point can only be at 9 positions relative to the
centre point of the tool tip radius. This has very little to do with
the flank angles. It is more related to which quadrants of a notional
full-circle tool are in use.
For example orienation 2 (right hand facing and turning) expects to be
touching at 12-o-clock when moving purely in Z and at 9-o-clock when
facing in X. If moving in some combination then the tool will be moved
a little bit closer to the work to compensate for the gap between the
controlled point and the tool tip that exists between those two
tangents.

For the vast majority of lathe work cutter comp is not important. The
positions of  shoulders and absolute diameters are unaffected. Tapers
will end up a little fatter than drawn and both external and internal
fillets will have extra material. The latter vary rarely matters, and
the former normally seem to need some tweaking-to-fit anyway, so I run
with cutter-comp turned off nearly all the time.
If I was machining accurate spheres then things would be different.


-- 
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, 1916

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 22:39:18 Ken Strauss wrote:

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: Sunday, August 05, 2018 10:27 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > Thats a sweet idea, but all holders would appear to be made to fit
> > that custom spindle. So the whole thing would need at least a little
> > red wagon full of rolls of SBA dollars. Good for a new design, sure,
> > but would obsolete $2000+ dollars worth of tool holders I already
> > have. The carousel could be made to fit the TTS holders easy enough,
> > but what about a tool that doesn't fit a 3/4" r8?. Show stopper.
> > Needs more thought to make it a bit more universal.
>
> I have a PDB and only use TTS tooling so changing tooling would not be
> problem. With only 1HP to the spindle there is little reason for me to
> use cutters with a shank larger than 3/4-inch.
>
Particularly if you raise the motor power, the TTS may slip in its holder 
as it has no provision to keylock it to the spindle. It seriously needs 
a keying slot cut into the side, and a locking pin to engage that slot 
in the spindle. When I went of a spree and cut up 12 feet of 7/8" brass 
for tap holders, I skipped the TTS and cut a semi-circle to fit the head 
of a 4mm socket head cap screw into the edge of a 7/8" r8 so the tap is 
keyed into the r8, which is keyed into my spindle. zero tap  slippage 
now. An er20 takes 18" wrenches tightened seriously to get a good enough 
grip on a 4mm.7 tap. With my psu and a Pico pwm-servo amp, I'm getting 
close to 2hp out of the factory G0704 motor.  Its almost enough to turn 
a 12mm tap in steel.  And will get the job done if I "peck" it.  How 
long those plastic backgears would last doing that is Yet To Be 
Determined. :)
>
> --
> Check out the vibrant tech community on one of the world's
> most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> 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)
Genes Web page <http://geneslinuxbox.net:6309/gene>

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Ken Strauss]

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, August 05, 2018 10:27 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] Cutter compensation with mill turning
>
> Thats a sweet idea, but all holders would appear to be made to fit that
> custom spindle. So the whole thing would need at least a little red
> wagon full of rolls of SBA dollars. Good for a new design, sure, but
> would obsolete $2000+ dollars worth of tool holders I already have. The
> carousel could be made to fit the TTS holders easy enough, but what
> about a tool that doesn't fit a 3/4" r8?. Show stopper. Needs more
> thought to make it a bit more universal.
> >

I have a PDB and only use TTS tooling so changing tooling would not be
problem. With only 1HP to the spindle there is little reason for me to use
cutters with a shank larger than 3/4-inch.



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 18:03:53 andy pugh wrote:

> On 5 August 2018 at 19:31, Gene Heskett  wrote:
> > Are these angles to be expressed as the angle from the chip
> > centerline, or in an absolute angle assuming 0 degrees is exactly
> > away from the operator?
>
> Neither.
> They are the angles of the tool flanks from a zero-degree line that
> extends along the Z axis.
>
> (The diagram of the tool orientations does include some front and back
> angles to clarify this point)
>
That did not bite me on the ankle Andy.  Thanks for the clue, but it 
really needs to be in the text of the Doc.pdf.

> At the moment the angles are only used by the Axis preview, so you
> don't really need to be too fussy about them.

Tool paths (corrected) are I assume to be the nearest of the 8 positions, 
or are those actually calculated from data in the tool table (and fussed 
about if obviously wrong I hope.  This, not having tried it, has 
obviously not been tested)

> In the future, when TypeII G71 is properly introduced then the angles
> will be used for gouge-prevention.
>
> (Already working in the Python mockup)

Great! Do carry on then ;-) In 2.8.0 final?

Thanks Andy.

-- 
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)
Genes Web page 

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 17:03:42 Ken Strauss wrote:

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: Sunday, August 05, 2018 2:31 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > On Sunday 05 August 2018 13:43:45 Ken Strauss wrote:
> > > > -Original Message-
> > > > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > > > Sent: Sunday, August 05, 2018 12:57 PM
> > > > To: emc-users@lists.sourceforge.net
> > > > Subject: Re: [Emc-users] Cutter compensation with mill turning
> > > >
> > > > On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:
> > > >
> > > > Looking at the drawings for position 9, page 78 of 738, I too am
> > > > confused. Can we be enlightened? IMO there are only 8 usable
> > > > positions. Which in the practical world, none are 100% accurate
> > > > because no one sets up a tool with the full side of its cutting
> > > > edge inline with either axis. Thats just asking for and usually
> > > > getting a squeak/chatter and a broken insert.
> > >
> > > The I/J parameters on a G10 L1 allow the specification of the
> > > FRONTANGLE and BACKANGLE shown in the drawing. I'm guessing that
> > > 30-degrees is the default for these angles.
> >
> > Are these angles to be expressed as the angle from the chip
> > centerline, or in an absolute angle assuming 0 degrees is exactly
> > away from the operator? Little but very important details are not
> > adequately discussed, and that has discouraged my use of the tool
> > table.
>
> From the illustration at the very end of
> http://wiki.linuxcnc.org/cgi-bin/wiki.pl?ToolTable it appears that
> FRONTANGLE and BACKANGLE are measured from the centre line of the
> tool.
>
> > Lack of a tool changer has also discouraged it, but thats my fault.
> > Every design I have seen, and have been tempted to make, also wants
> > to impinge on the operating envelope in ways its hard to work
> > around. So 3 or so holders along the end of the table are out, as
> > are those I've seen along the back edge of the table. Neither are
> > practical from the standpoint of the uneven weight on the end of the
> > table.
>
> I would also like an ATC but have balked at Tormach's price for such.
> Tools for my size machine typically weigh far less than a pound each
> so I'm not particularly concerned about the uneven weight. However,
> not losing table space is critical. A changer with only four or five
> tool holders would suffice for most of my work. There are several
> simple designs such as https://www.youtube.com/watch?v=s11izziBkbs
> that seem to be a possibility.

Thats a sweet idea, but all holders would appear to be made to fit that 
custom spindle. So the whole thing would need at least a little red 
wagon full of rolls of SBA dollars. Good for a new design, sure, but 
would obsolete $2000+ dollars worth of tool holders I already have. The 
carousel could be made to fit the TTS holders easy enough, but what 
about a tool that doesn't fit a 3/4" r8?. Show stopper. Needs more 
thought to make it a bit more universal.
>
>
> --
> Check out the vibrant tech community on one of the world's
> most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> 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)
Genes Web page <http://geneslinuxbox.net:6309/gene>

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 13:43:45 Ken Strauss wrote:

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: Sunday, August 05, 2018 12:57 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:
> >
> > Looking at the drawings for position 9, page 78 of 738, I too am
> > confused. Can we be enlightened? IMO there are only 8 usable
> > positions. Which in the practical world, none are 100% accurate
> > because no one sets up a tool with the full side of its cutting edge
> > inline with either axis. Thats just asking for and usually getting a
> > squeak/chatter and a broken insert.
>
> The I/J parameters on a G10 L1 allow the specification of the
> FRONTANGLE and BACKANGLE shown in the drawing. I'm guessing that
> 30-degrees is the default for these angles.

But, from what reference is that +-30 degrees measured? Are we talking 
true, as in 0 degrees means its pointed straight away from the operator 
+-30 degrees? Or are we assuming a 30 degree angle measured from the 
tools actual orientation, which ack the Doc.pdf, is every 45 degrees 
around the compass? It seems to me that rather than 8 arbitrary 
positions, it should have been specced in degrees, with 0 up or away.  
The math to draw the backplot correctly would have been no more complex 
than it is now, and the 1 to 8 lookup table used to convert the 1 t8 
into a real angle, could probably just go away.

Thanks.

-- 
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)
Genes Web page <http://geneslinuxbox.net:6309/gene>

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[andy pugh]

On 5 August 2018 at 19:31, Gene Heskett  wrote:

> Are these angles to be expressed as the angle from the chip centerline,
> or in an absolute angle assuming 0 degrees is exactly away from the
> operator?

Neither.
They are the angles of the tool flanks from a zero-degree line that
extends along the Z axis.

(The diagram of the tool orientations does include some front and back
angles to clarify this point)

At the moment the angles are only used by the Axis preview, so you
don't really need to be too fussy about them.

In the future, when TypeII G71 is properly introduced then the angles
will be used for gouge-prevention.

(Already working in the Python mockup)

-- 
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, 1916

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Ken Strauss]

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, August 05, 2018 2:31 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] Cutter compensation with mill turning
>
> On Sunday 05 August 2018 13:43:45 Ken Strauss wrote:
>
> > > -Original Message-
> > > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > > Sent: Sunday, August 05, 2018 12:57 PM
> > > To: emc-users@lists.sourceforge.net
> > > Subject: Re: [Emc-users] Cutter compensation with mill turning
> > >
> > > On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:
> > >
> > > Looking at the drawings for position 9, page 78 of 738, I too am
> > > confused. Can we be enlightened? IMO there are only 8 usable
> > > positions. Which in the practical world, none are 100% accurate
> > > because no one sets up a tool with the full side of its cutting edge
> > > inline with either axis. Thats just asking for and usually getting a
> > > squeak/chatter and a broken insert.
> >
> > The I/J parameters on a G10 L1 allow the specification of the
> > FRONTANGLE and BACKANGLE shown in the drawing. I'm guessing that
> > 30-degrees is the default for these angles.
> >
> Are these angles to be expressed as the angle from the chip centerline,
> or in an absolute angle assuming 0 degrees is exactly away from the
> operator? Little but very important details are not adequately
> discussed, and that has discouraged my use of the tool table.
>

>From the illustration at the very end of
http://wiki.linuxcnc.org/cgi-bin/wiki.pl?ToolTable it appears that
FRONTANGLE and BACKANGLE are measured from the centre line of the tool.

> Lack of a tool changer has also discouraged it, but thats my fault. Every
> design I have seen, and have been tempted to make, also wants to impinge
> on the operating envelope in ways its hard to work around. So 3 or so
> holders along the end of the table are out, as are those I've seen along
> the back edge of the table. Neither are practical from the standpoint of
> the uneven weight on the end of the table.
>
I would also like an ATC but have balked at Tormach's price for such. Tools
for my size machine typically weigh far less than a pound each so I'm not
particularly concerned about the uneven weight. However, not losing table
space is critical. A changer with only four or five tool holders would
suffice for most of my work. There are several simple designs such as
https://www.youtube.com/watch?v=s11izziBkbs that seem to be a possibility.



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 13:43:45 Ken Strauss wrote:

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: Sunday, August 05, 2018 12:57 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:
> >
> > Looking at the drawings for position 9, page 78 of 738, I too am
> > confused. Can we be enlightened? IMO there are only 8 usable
> > positions. Which in the practical world, none are 100% accurate
> > because no one sets up a tool with the full side of its cutting edge
> > inline with either axis. Thats just asking for and usually getting a
> > squeak/chatter and a broken insert.
>
> The I/J parameters on a G10 L1 allow the specification of the
> FRONTANGLE and BACKANGLE shown in the drawing. I'm guessing that
> 30-degrees is the default for these angles.
>
Are these angles to be expressed as the angle from the chip centerline, 
or in an absolute angle assuming 0 degrees is exactly away from the 
operator? Little but very important details are not adequately 
discussed, and that has discouraged my use of the tool table.

Lack of a tool changer has also discouraged it, but thats my fault. Every 
design I have seen, and have been tempted to make, also wants to impinge 
on the operating envelope in ways its hard to work around. So 3 or so 
holders along the end of the table are out, as are those I've seen along 
the back edge of the table. Neither are practical from the standpoint of 
the uneven weight on the end of the table.

And when thats worked around by assuming an intermediate tool transfer 
arm, controlling such a beast isn't trivial because either it or the 
tool carrying carousel also has to have either a slide in and out 
gripper, or a z drive of its own. And it also needs to have effective 
swarf shielding when its swung out of the way of the heads own z 
motions.

The final idea killer is that within reason, a 2 armed tool changer (me) 
is still practical because what I do doesn't generate an income anyway. 
And its an r8 spindle, so the electric driver with a ratcheting hammer 
drive on the draw bar also needs to be positioned on the drawbar bolt 
and driven. One of the cats with an air drive would be tons simpler to 
control. I did find a source of 5/16" 8 point sockets and bought a small 
bag of them, so I'm no longer worried about splitting the one in current 
use. That Porter-Cable driver is a serious driver, and will eventually 
finish off the current socket.

I'll have to admit it would be nice to impress the visiting frogs with 
though. :)

>
>
> --
> Check out the vibrant tech community on one of the world's
> most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> 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)
Genes Web page <http://geneslinuxbox.net:6309/gene>

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Ken Strauss]

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, August 05, 2018 12:57 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] Cutter compensation with mill turning
>
> On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:
>
> Looking at the drawings for position 9, page 78 of 738, I too am
> confused. Can we be enlightened? IMO there are only 8 usable positions.
> Which in the practical world, none are 100% accurate because no one sets
> up a tool with the full side of its cutting edge inline with either
> axis. Thats just asking for and usually getting a squeak/chatter and a
> broken insert.

The I/J parameters on a G10 L1 allow the specification of the FRONTANGLE and
BACKANGLE shown in the drawing. I'm guessing that 30-degrees is the default
for these angles.



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 09:33:22 andy pugh wrote:

> On 5 August 2018 at 14:07, Ken Strauss  wrote:
> > I had looked at
> > http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_
> >orientation_a_id_lathe_tool_orientation_a but obviously not
> > understood the drawing. Is "Position 9" the controlled point? I
>
> No, position 9 is a round "button" tool.
>
So for position 9 we would enter the radii of the button? It is a 
tooltype I don't own.

I'd also make the comment that it sure would be nice, and usefull, if the 
tip radii was listed on the little plastic boxes the inserts usually 
come in. It takes entirely too long to locate that information on the 
chip makers web site.

> The controlled point is the red cross on each position. Only position
> 9 has the controlled point inside the tool material.

Which leads to an interesting train of thought, and I may yet buy such a 
tool holder.


-- 
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)
Genes Web page 

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Sunday 05 August 2018 09:07:29 Ken Strauss wrote:

> To clarify:
> As Gene mentioned I intended to type "G18 (XZ plane)"
> I am not using straight LinuxCNC but Tormach's adaptation that they
> call PathPilot. They have different versions for lathe and mill that I
> believe change the INI file as Andy mentioned. I was planning to use
> the mill version. The parts that I am trying to make include both
> tapers and curves so the tool orientation matters.
>
> I had looked at
> http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_or
>ientation_a_id_lathe_tool_orientation_a but obviously not understood
> the drawing. Is "Position 9" the controlled point? If I use G10 L1 in
> mill mode are the I/J/Q parameters ignored in subsequent commands?
>
Looking at the drawings for position 9, page 78 of 738, I too am 
confused. Can we be enlightened? IMO there are only 8 usable positions. 
Which in the practical world, none are 100% accurate because no one sets 
up a tool with the full side of its cutting edge inline with either 
axis. Thats just asking for and usually getting a squeak/chatter and a 
broken insert.

> > -Original Message-
> > From: andy pugh [mailto:bodge...@gmail.com]
> > Sent: Sunday, August 05, 2018 7:52 AM
> > To: Enhanced Machine Controller (EMC)
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > On 5 August 2018 at 04:31, Ken Strauss  wrote:
> > > I want to use mill turning using hand written code and I am
> > > confused about cutter compensation.
> >
> > Is this using the mill spindle as the spindle, or using a subsidiary
> > spindle?
> >
> > > Is the controlled point at the centre of a circle specified by the
> > > D parameter?
> >
> > With a lathe tool the controlled point is typically _outside_ the
> > tool. Without compensation you will normally get accurate faces and
> > diameters, the compensation only really becomes relevant for curves
> > and tapers.
> >
> > The controlled points are shown here:
> > http://linuxcnc.org/docs/2.7/html/lathe/lathe-
> > user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
> >
> > I do not know how the system knows whether to use lathe or mill
> > style radius compensation. It might be based on the LATHE=1 in the
> > INI, or it might be done on a tool-by-tool basis using the tool
> > table. For mill-turn the latter option would be more helpful.
> >
> > --
> > 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, 1916
> >
> > 
> >-- Check out the vibrant tech community on one of the world's
> > most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
> --
> Check out the vibrant tech community on one of the world's
> most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> 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)
Genes Web page <http://geneslinuxbox.net:6309/gene>

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[andy pugh]

On 5 August 2018 at 14:07, Ken Strauss  wrote:

> I had looked at
> http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
> but obviously not understood the drawing. Is "Position 9" the controlled
> point? I

No, position 9 is a round "button" tool.

The controlled point is the red cross on each position. Only position
9 has the controlled point inside the tool material.

-- 
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, 1916

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Stuart Stevenson]

In any orientation the calculations must use the center of the cutter
radius. This applies to milling and turning. Cutter compensation must know
the corner radius when using a turning insert and the cutter radius when
milling.

On Sun, Aug 5, 2018, 8:08 AM Ken Strauss  wrote:

> To clarify:
> As Gene mentioned I intended to type "G18 (XZ plane)"
> I am not using straight LinuxCNC but Tormach's adaptation that they call
> PathPilot. They have different versions for lathe and mill that I believe
> change the INI file as Andy mentioned. I was planning to use the mill
> version.
> The parts that I am trying to make include both tapers and curves so the
> tool
> orientation matters.
>
> I had looked at
>
> http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
> but obviously not understood the drawing. Is "Position 9" the controlled
> point? If I use G10 L1 in mill mode are the I/J/Q parameters ignored in
> subsequent commands?
>
> > -Original Message-
> > From: andy pugh [mailto:bodge...@gmail.com]
> > Sent: Sunday, August 05, 2018 7:52 AM
> > To: Enhanced Machine Controller (EMC)
> > Subject: Re: [Emc-users] Cutter compensation with mill turning
> >
> > On 5 August 2018 at 04:31, Ken Strauss  wrote:
> > > I want to use mill turning using hand written code and I am confused
> about
> > > cutter compensation.
> >
> > Is this using the mill spindle as the spindle, or using a subsidiary
> > spindle?
> >
> > > Is the controlled point at the centre of a circle specified by the D
> > > parameter?
> >
> > With a lathe tool the controlled point is typically _outside_ the tool.
> > Without compensation you will normally get accurate faces and
> > diameters, the compensation only really becomes relevant for curves
> > and tapers.
> >
> > The controlled points are shown here:
> > http://linuxcnc.org/docs/2.7/html/lathe/lathe-
> > user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
> >
> > I do not know how the system knows whether to use lathe or mill style
> > radius compensation. It might be based on the LATHE=1 in the INI, or
> > it might be done on a tool-by-tool basis using the tool table.
> > For mill-turn the latter option would be more helpful.
> >
> > --
> > 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, 1916
> >
> >
> --
> > Check out the vibrant tech community on one of the world's most
> > engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
>
> --
> Check out the vibrant tech community on one of the world's most
> engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>
--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Ken Strauss]

To clarify:
As Gene mentioned I intended to type "G18 (XZ plane)"
I am not using straight LinuxCNC but Tormach's adaptation that they call 
PathPilot. They have different versions for lathe and mill that I believe 
change the INI file as Andy mentioned. I was planning to use the mill version. 
The parts that I am trying to make include both tapers and curves so the tool 
orientation matters.

I had looked at 
http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
 
but obviously not understood the drawing. Is "Position 9" the controlled 
point? If I use G10 L1 in mill mode are the I/J/Q parameters ignored in 
subsequent commands?

> -Original Message-
> From: andy pugh [mailto:bodge...@gmail.com]
> Sent: Sunday, August 05, 2018 7:52 AM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Cutter compensation with mill turning
>
> On 5 August 2018 at 04:31, Ken Strauss  wrote:
> > I want to use mill turning using hand written code and I am confused about
> > cutter compensation.
>
> Is this using the mill spindle as the spindle, or using a subsidiary 
> spindle?
>
> > Is the controlled point at the centre of a circle specified by the D
> > parameter?
>
> With a lathe tool the controlled point is typically _outside_ the tool.
> Without compensation you will normally get accurate faces and
> diameters, the compensation only really becomes relevant for curves
> and tapers.
>
> The controlled points are shown here:
> http://linuxcnc.org/docs/2.7/html/lathe/lathe-
> user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a
>
> I do not know how the system knows whether to use lathe or mill style
> radius compensation. It might be based on the LATHE=1 in the INI, or
> it might be done on a tool-by-tool basis using the tool table.
> For mill-turn the latter option would be more helpful.
>
> --
> 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, 1916
>
> --
> Check out the vibrant tech community on one of the world's most
> engaging tech sites, Slashdot.org! http://sdm.link/slashdot
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[andy pugh]

On 5 August 2018 at 04:31, Ken Strauss  wrote:
> I want to use mill turning using hand written code and I am confused about
> cutter compensation.

Is this using the mill spindle as the spindle, or using a subsidiary spindle?

> Is the controlled point at the centre of a circle specified by the D
> parameter?

With a lathe tool the controlled point is typically _outside_ the tool.
Without compensation you will normally get accurate faces and
diameters, the compensation only really becomes relevant for curves
and tapers.

The controlled points are shown here:
http://linuxcnc.org/docs/2.7/html/lathe/lathe-user.html#_lathe_tool_orientation_a_id_lathe_tool_orientation_a

I do not know how the system knows whether to use lathe or mill style
radius compensation. It might be based on the LATHE=1 in the INI, or
it might be done on a tool-by-tool basis using the tool table.
For mill-turn the latter option would be more helpful.

-- 
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, 1916

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Cutter compensation with mill turning

[Gene Heskett]

On Saturday 04 August 2018 23:31:44 Ken Strauss wrote:

> I want to use mill turning using hand written code and I am confused
> about cutter compensation.
>
> If I select the ZX plane (G17) and use G41.1/G42.1, is the L parameter
> acted upon? Is the controlled point at the centre of a circle
> specified by the D parameter?
>
First G17 is std XY on a mill. So I'm a bit confused.

Second, I generally write my own code and use the tools radii as the 
controlled point. But read the man pages for G41.1/G42.1. You may 
understand it better than I do. The diff between g42 and g42.1 is that 
g42 gets the offset from the tool table, whereas g42.1 offset comes from 
your entry in the code. Ditto for g41/g41.1.

In these cases, I always install the docs for the release I'm running, 
normally master.  Than its no farther away than:

okteta /usr/share/doc/linuxcnc/Documentation_LinuxCNC.pdf

I Hope this helps.


> Thanks in advance for any help.

-- 
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)
Genes Web page 

--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] Cutter compensation with mill turning

[Ken Strauss]

I want to use mill turning using hand written code and I am confused about
cutter compensation.

If I select the ZX plane (G17) and use G41.1/G42.1, is the L parameter acted
upon? Is the controlled point at the centre of a circle specified by the D
parameter?

Thanks in advance for any help.



--
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users