[Emc-users] Using a mill as a lathe, EMC2 implications

[Igor Chudov]

I have a Bridgeport Interact CNC mill.

Yesterday, I attached a 3 inch lathe chuck to a QC-30 tool holder, so
I can use this mill as a CNC lathe, without the tailstock of course. I
would hold the lathe bit in the vise.

Even without a tailstock, I consider this to be a pretty useful
project, basically adding a CNC lathe like an OmniTurn, without really
having a separate machine. I can make curvy things on this setup. I
have a manual lathe, for big stuff, but for small intricate curvy
projects, I can use the Bridgeport mill with lathe chuck.

But my question is EMC2 settings and how I can use EMC2 in ways that
are more lathe specific. Ultimately I want to write a subroutine that
would change settings to be more lathe-like and another sub that
changes settings back to more mill-like.

So... what makes a lathe different from a mill? One thing that comes
to mins is to use XZ plane for circles. That way, I can mill ball ends
and such, using G2 and G3.

Anything else? Any other commands that set myself up for single point turning?

[Kirk Wallace]

On Mon, 2010-11-15 at 10:43 -0600, Igor Chudov wrote:
... snip
> So... what makes a lathe different from a mill? One thing that comes
> to mins is to use XZ plane for circles. That way, I can mill ball ends
> and such, using G2 and G3.
>
> Anything else? Any other commands that set myself up for single point turning?

In case it hasn't be considered yet, there is an .ini setting for
lathes, in the DISPLAY section:
http://www.linuxcnc.org/docview/html//config_ini_config.html#sub:%5BDISPLAY%5D-section
(Short URL) http://alturl.com/gb3fx

(Just load either the mill or lathe .ini file at the EMC2 start-up prompt.)

Also:
http://wiki.linuxcnc.org/emcinfo.pl?Lathe_Advanced_Features

I guess Y will become tool height, also guessing that you'll set Y with
the manual mode, and leave Y out of your g-code (unless you want to get
creative).

The tool table is different:
http://linuxcnc.org/docs/html/lathe_lathe-user.html#r1_2

You'll need to set this in the .ini file too:
http://www.linuxcnc.org/docview/html//config_ini_config.html#sub:%5BEMCIO%5D-Section
(Short URL) http://alturl.com/jwjkg

That's what comes to mind so far, hopefully someone with actual
experience will chime in.

--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[Andy Pugh]

On 15 November 2010 16:43, Igor Chudov <***@gmail.com> wrote:

> But my question is EMC2 settings and how I can use EMC2 in ways that
> are more lathe specific.

I have a machine which is both a lathe and a mill.
I just use two sets of config files, so that the right Axis values go
to the right stepgens. What the machine is depends on which icon I
click.

In my case Mill X becomes Lathe Z, mill Y becomes Lathe X, Mill Z is unused.

In your case the actual X and Z mappings stay the same. I am not sure
if you can have a Y axis in a lathe config, but you could potentially
link Y to a "tool height" pyvcp box.

--
atp

[Igor Chudov]

Andy and Kirk, thanks a lot.

How is Z set up on lathe: does Z increase as I get closer to the lathe chuck?

Anyway, my first project would be to make a round (ball) end to a
presently square end cylinder. I, obviously, cannot do it in one cut
due to rigidity. So I would need to make several passes.

Is there a canned cycle or some available subroutine to do so?

Igor

On Mon, Nov 15, 2010 at 11:22 AM, Andy Pugh <***@andypugh.fsnet.co.uk> wrote:
> On 15 November 2010 16:43, Igor Chudov <***@gmail.com> wrote:
>
>> But my question is EMC2 settings and how I can use EMC2 in ways that
>> are more lathe specific.
>
> I have a machine which is both a lathe and a mill.
> I just use two sets of config files, so that the right Axis values go
> to the right stepgens. What the machine is depends on which icon I
> click.
>
> In my case Mill X becomes Lathe Z, mill Y becomes Lathe X, Mill Z is unused.
>
> In your case the actual X and Z mappings stay the same. I am not sure
> if you can have a Y axis in a lathe config, but you could potentially
> link Y to a "tool height" pyvcp box.
>
> --
> atp
>
> ------------------------------------------------------------------------------
> Centralized Desktop Delivery: Dell and VMware Reference Architecture
> Simplifying enterprise desktop deployment and management using
> Dell EqualLogic storage and VMware View: A highly scalable, end-to-end
> client virtualization framework. Read more!
> http://p.sf.net/sfu/dell-eql-dev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

[Andy Pugh]

On 15 November 2010 17:29, Igor Chudov <***@gmail.com> wrote:

> How is Z set up on lathe: does Z increase as I get closer to the lathe chuck?

No, it decreases. You spend a lot of time cutting negative numbers.
In G7 mode you work in diamter, not X, by the way.

> Anyway, my first project would be to make a round (ball) end to a
> presently square end cylinder. I, obviously, cannot do it in one cut
> due to rigidity. So I would need to make several passes.
>
> Is there a canned cycle or some available subroutine to do so?

No, but it would be an easy WHILE loop. You can use G2 and G3 in the G18 plane.

--
atp

[Jon Elson]

Igor Chudov wrote:
> Andy and Kirk, thanks a lot.
>
> How is Z set up on lathe: does Z increase as I get closer to the lathe chuck?
>
No, the RS274-D definition is the same, moving the tool toward the chuck
is -Z.
>
> Is there a canned cycle or some available subroutine to do so?
>
I have attached a C program that I used for my ball turning. I see some
comments that indicate it
was adapted from a different program, and these comments probably no
longer make sense.

Jon

[Igor Chudov]

Thanks for the program Jon. I will try to understand it and maybe use
as a basis for a G code sub.

I will try to do it so that I could make ball ends spanning more than
180 degrees.

One more question: when making a part without a tailstock, I have to
be double sure that the part is as rigid at any moment as possible.
So, it would make sense to program things to use something like a
cutoff bit to rough out the part by removing as much material on the
farthest end as possible, and then moving slightly close to the chuck
and repeating. As opposed to roughing by running along Z many times.

Is that making any sense?

i

On Mon, Nov 15, 2010 at 12:33 PM, Jon Elson <***@pico-systems.com> wrote:
> Igor Chudov wrote:
>>
>> Andy and Kirk, thanks a lot.
>>
>> How is Z set up on lathe: does Z increase as I get closer to the lathe
>> chuck?
>>
>
> No, the RS274-D definition is the same, moving the tool toward the chuck is
> -Z.
>>
>> Is there a canned cycle or some available subroutine to do so?
>>
>
> I have attached a C program that I used for my ball turning.  I see some
> comments that indicate it
> was adapted from a different program, and these comments probably no longer
> make sense.
>
> Jon
>
> ------------------------------------------------------------------------------
> Centralized Desktop Delivery: Dell and VMware Reference Architecture
> Simplifying enterprise desktop deployment and management using
> Dell EqualLogic storage and VMware View: A highly scalable, end-to-end
> client virtualization framework. Read more!
> http://p.sf.net/sfu/dell-eql-dev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>
>

[Jon Elson]

Igor Chudov wrote:
> Thanks for the program Jon. I will try to understand it and maybe use
> as a basis for a G code sub.
>
> I will try to do it so that I could make ball ends spanning more than
> 180 degrees.
>
>
If I understand you correctly, cutting 180 degrees of the ball will
cause it to fall off
the stock.
> One more question: when making a part without a tailstock, I have to
> be double sure that the part is as rigid at any moment as possible.
> So, it would make sense to program things to use something like a
> cutoff bit to rough out the part by removing as much material on the
> farthest end as possible, and then moving slightly close to the chuck
> and repeating. As opposed to roughing by running along Z many times.
>
I used only one tool, I said in an earlier message it was a triangular
insert, I now remember I
used a round insert, it made the setup and programming much easier. I
programmed it
with the center of the insert in mind. I did an arc that moves closer
on each pass. It might
have taken just a minute longer than an intelligent code that doesn't
cut air, but it really
wasn't bad at all.

Jon

[Igor Chudov]

On Tue, Nov 16, 2010 at 12:01 AM, Jon Elson <***@pico-systems.com> wrote:
> Igor Chudov wrote:
>> Thanks for the program Jon. I will try to understand it and maybe use
>> as a basis for a G code sub.
>>
>> I will try to do it so that I could make ball ends spanning more than
>> 180 degrees.
>>
>>
> If I understand you correctly, cutting 180 degrees of the ball will
> cause it to fall off
> the stock.

The way I think, 180 degrees makes a half ball, and 360 makes a full
ball (and would cause it to fall of as you said).

So I would like to write code that is capable of cutting more than
180, but less than 360 degrees.

>> One more question: when making a part without a tailstock, I have to
>> be double sure that the part is as rigid at any moment as possible.
>> So, it would make sense to program things to use something like a
>> cutoff bit to rough out the part by removing as much material on the
>> farthest end as possible, and then moving slightly close to the chuck
>> and repeating. As opposed to roughing by running along Z many times.
>>
> I used only one tool, I said in an earlier message it was a triangular
> insert, I now remember I
> used a round insert, it made the setup and programming much easier.  I
> programmed it
> with the center of the insert in mind.  I did an arc that moves closer
> on each pass.  It might
> have taken just a minute longer than an intelligent code that doesn't
> cut air, but it really
> wasn't bad at all.

Sounds great. Thanks Jon. This is very exciting, like getting a new machine.

i

[Andy Pugh]

On 16 November 2010 12:50, Igor Chudov <***@gmail.com> wrote:

> So I would like to write code that is capable of cutting more than
> 180, but less than 360 degrees.

The code I posted will cut any angle up to 360. Try it :-)

--
atp

[Igor Chudov]

Yep, I will definitely try it, thanks Andy.

I would really love to see a small improvement of EMC capabilities
that would allow people to create packaged G code libraries. The
capability is searching through a load PATH.

Igor

On Tue, Nov 16, 2010 at 7:31 AM, Andy Pugh <***@andypugh.fsnet.co.uk> wrote:
> On 16 November 2010 12:50, Igor Chudov <***@gmail.com> wrote:
>
>> So I would like to write code that is capable of cutting more than
>> 180, but less than 360 degrees.
>
> The code I posted will cut any angle up to 360. Try it :-)
>
> --
> atp
>
> ------------------------------------------------------------------------------
> Beautiful is writing same markup. Internet Explorer 9 supports
> standards for HTML5, CSS3, SVG 1.1,  ECMAScript5, and DOM L2 & L3.
> Spend less time writing and  rewriting code and more time creating great
> experiences on the web. Be a part of the beta today
> http://p.sf.net/sfu/msIE9-sfdev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

[Dewey Garrett]

>I would really love to see a small improvement of EMC capabilities
>that would allow people to create packaged G code libraries. The
>capability is searching through a load PATH.


In git master, you can specify a search path for subroutines with
[RS274NGC]SUBROUTINE_PATH

see:
http://git.linuxcnc.org/gitweb?p=emc2.git;a=commitdiff;h=0a5f2ca6f9f0793c895b8c5e4ade6e2681f910b3

and
http://git.linuxcnc.org/gitweb?p=emc2.git;a=commitdiff;h=81a6dce8410df3097387a8745fd2a11f76fe4941

and Section 4.2.4 of
http://linuxcnc.org/docs/devel/EMC2_Integrator_Manual.pdf

dewey
--
Dewey Garrett

[Igor Chudov]

This is most outstanding, I am delighted to see this.

That way I can keep stuff in places where it belongs, as opposed to
one junk pile.

Thank you!

Igor

On Tue, Nov 16, 2010 at 12:12 PM, Dewey Garrett <***@panix.com> wrote:
>
>>I would really love to see a small improvement of EMC capabilities
>>that would allow people to create packaged G code libraries. The
>>capability is searching through a load PATH.
>
>
> In git master, you can specify a search path for subroutines with
>    [RS274NGC]SUBROUTINE_PATH
>
> see:
> http://git.linuxcnc.org/gitweb?p=emc2.git;a=commitdiff;h=0a5f2ca6f9f0793c895b8c5e4ade6e2681f910b3
>
> and
> http://git.linuxcnc.org/gitweb?p=emc2.git;a=commitdiff;h=81a6dce8410df3097387a8745fd2a11f76fe4941
>
> and  Section 4.2.4 of
> http://linuxcnc.org/docs/devel/EMC2_Integrator_Manual.pdf
>
> dewey
> --
> Dewey Garrett
>
>
> ------------------------------------------------------------------------------
> Beautiful is writing same markup. Internet Explorer 9 supports
> standards for HTML5, CSS3, SVG 1.1,  ECMAScript5, and DOM L2 & L3.
> Spend less time writing and  rewriting code and more time creating great
> experiences on the web. Be a part of the beta today
> http://p.sf.net/sfu/msIE9-sfdev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

[Jon Elson]

Igor Chudov wrote:
> The way I think, 180 degrees makes a half ball, and 360 makes a full
> ball (and would cause it to fall of as you said).
>
> So I would like to write code that is capable of cutting more than
> 180, but less than 360 degrees.
>
OK, your description is consistent. When I think of this, I think in
the toolpath frame
of reference, so a 180 degree move is moving the tool 180 degrees around
the arc.
>
> Sounds great. Thanks Jon. This is very exciting, like getting a new machine.
>
Yes, it was a quick, slap-dash thing for something I have only rare
occasion to do,
and I STILL have not gotten around to CNC-ing my lathe.

Jon

[Andy Pugh]

On 16 November 2010 16:58, Jon Elson <***@pico-systems.com> wrote:

> and I STILL have not gotten around to CNC-ing my lathe.

It's very worthwhile. Apart from anything else you get accuracy in Z
as well as X. Even without writing G-code with a few macros defined
you can set it off to turn down the work by .5" in 20thou steps for a
6" length and just leave it to it. Save a lot of time where the only
entertainment is picking hot swarf out of your collar.

Also, threading suddenly becomes trivial. And you can do things like
to 15.75mm x 0.6mm thread that I used to hold parts of my drawbar
together, because CNC doesn't care what changewheels you have.

--
atp

[Igor Chudov]

On Tue, Nov 16, 2010 at 11:19 AM, Andy Pugh <***@andypugh.fsnet.co.uk> wrote:
> On 16 November 2010 16:58, Jon Elson <***@pico-systems.com> wrote:
>
>> and I STILL have not gotten around to CNC-ing my lathe.
>
> It's very worthwhile. Apart from anything else you get accuracy in Z
> as well as X. Even without writing G-code with a few macros defined
> you can set it off to turn down the work by .5" in 20thou steps for a
> 6" length and just leave it to it. Save a lot of time where the only
> entertainment is picking hot swarf out of your collar.
>
> Also, threading suddenly becomes trivial. And you can do things like
> to 15.75mm x 0.6mm thread that I used to hold parts of my drawbar
> together, because CNC doesn't care what changewheels you have.

So, Andy, what is involved? Changing leadscrews to ball screws and
adding servos etc?

Are ball screws easy to find? Say, I have a 14x48" lathe.


i

[Andy Pugh]

On 16 November 2010 17:36, Igor Chudov <***@gmail.com> wrote:

> So, Andy, what is involved? Changing leadscrews to ball screws and
> adding servos etc?

Z is very easy, you can easily fit a servo or stepper motor anywhere
convenient at either end of the bed.

You probably want to replace the entire apron. The ideal retrofit
candidate would be a lathe with a smashed or missing apron. I confess
I am not sure I would have the heart to retrofit a good, working,
lathe.

X is more tricky, there tends to be limited space for the nut, and
mounting the motor is not that easy either.
A readily-available backlash-free right-angled drive would be a huge
help. I have spent some time considering ways to twist a toothed belt
drive.

The solution I came up with for my nasty lathe is here starting at post 15
http://www.cnczone.com/forums/mini_lathe/63621-mini_lathe_cross_slide_ballscrew_solutions-2.html

> Are ball screws easy to find? Say, I have a 14x48" lathe.

Yes, you can buy them by the foot. (at about $15 a foot)

--
atp

[Kirk Wallace]

On Tue, 2010-11-16 at 18:25 +0000, Andy Pugh wrote:
... snip
> > Are ball screws easy to find? Say, I have a 14x48" lathe.
>
> Yes, you can buy them by the foot. (at about $15 a foot)
>

Huh? I would guess ground double nut (for preload) 1.00" diameter Z ball
screw and nut at about $300 per foot. Then you need to add the precision
angular contact bearings to mount the screw.

This is my version of the project:
http://www.wallacecompany.com/cnc_lathe/

It has been on the back burner for a few years :(

--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[Igor Chudov]

Looks like a fun project, and good execution on the way, but possibly
too much to deal with for me personally.

I am very happy with the price/fun/benefit ratios of converting an
original CNC machine with a bad control to EMC. In my case a
Bridgeport Interact mill. So, when I find myself with extra time and
room on my hands, this will probably be the route to take.

i

On Tue, Nov 16, 2010 at 2:12 PM, Kirk Wallace
<***@wallacecompany.com> wrote:
> On Tue, 2010-11-16 at 18:25 +0000, Andy Pugh wrote:
> ... snip
>> > Are ball screws easy to find? Say, I have a 14x48" lathe.
>>
>> Yes, you can buy them by the foot. (at about $15 a foot)
>>
>
> Huh? I would guess ground double nut (for preload) 1.00" diameter Z ball
> screw and nut at about $300 per foot. Then you need to add the precision
> angular contact bearings to mount the screw.
>
> This is my version of the project:
> http://www.wallacecompany.com/cnc_lathe/
>
> It has been on the back burner for a few years :(
>
> --
> Kirk Wallace
> http://www.wallacecompany.com/machine_shop/
> http://www.wallacecompany.com/E45/index.html
> California, USA
>
>
> ------------------------------------------------------------------------------
> Beautiful is writing same markup. Internet Explorer 9 supports
> standards for HTML5, CSS3, SVG 1.1,  ECMAScript5, and DOM L2 & L3.
> Spend less time writing and  rewriting code and more time creating great
> experiences on the web. Be a part of the beta today
> http://p.sf.net/sfu/msIE9-sfdev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

[Kirk Wallace]

On Tue, 2010-11-16 at 14:21 -0600, Igor Chudov wrote:
> Looks like a fun project, and good execution on the way, but possibly
> too much to deal with for me personally.
>
> I am very happy with the price/fun/benefit ratios of converting an
> original CNC machine with a bad control to EMC. In my case a
> Bridgeport Interact mill. So, when I find myself with extra time and
> room on my hands, this will probably be the route to take.
>
> i

I really think the way to go is to convert an existing CNC lathe with
EMC2. All of the really expensive bits are there (ball screws, flood,
tool changer, collet closer, parts grabber, etcetra), installed and
proven to work. CNC lathes should be pretty cheap if you can find a way
to move it yourself. I'm only thinking of finishing my project, because
I sold some of the parts, and I want to finish what I started. I just
wish I had the knowledge I have now, before I took the lathe apart. But
if no one dies or gets hurt, it's all good. I _really_ want a robot.
--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[Igor Chudov]

On Tue, Nov 16, 2010 at 2:37 PM, Kirk Wallace
<***@wallacecompany.com> wrote:

> I really think the way to go is to convert an existing CNC lathe with
> EMC2. All of the really expensive bits are there (ball screws, flood,
> tool changer, collet closer, parts grabber, etcetra), installed and
> proven to work.

Yes, exactly. A machine originally designed for CNC, has all the
precision machining, parts fitting, vibration analysis, lubrication,
safeties, limits, drains, guards, servo motor mounts, ballscrews,
speed changing, etc etc etc etc etc all done and settled. The real
improvement would come from using a smart, PC based control instead of
some ancient piece of electronics that was on the machine originally.

My own retrofit project with the Bridgeport, involved almost zero
precision machining and parts fitting. The only exception was to make
encoder mounts for the servo motors. Everything else was reading,
asking questions and a lot of wiring work.

> CNC lathes should be pretty cheap if you can find a way
> to move it yourself. I'm only thinking of finishing my project, because
> I sold some of the parts, and I want to finish what I started. I just
> wish I had the knowledge I have now, before I took the lathe apart. But
> if no one dies or gets hurt, it's all good. I _really_ want a robot.

Yep. I wish I had room and time, I would definitely get a CNC lathe to
retrofit.

i

[Andy Pugh]

On 16 November 2010 20:21, Igor Chudov <***@gmail.com> wrote:

> I am very happy with the price/fun/benefit ratios of converting an
> original CNC machine with a bad control to EMC. In my case a
> Bridgeport Interact mill. So, when I find myself with extra time and
> room on my hands, this will probably be the route to take.

It is absolutely the best route to take. The only reason I am not
doing exactly that is that I don't have the space.

--
atp

[Andy Pugh]

On 16 November 2010 20:12, Kirk Wallace <***@wallacecompany.com> wrote:

>> Yes, you can buy them by the foot. (at about $15 a foot)
>
> Huh? I would guess ground double nut (for preload) 1.00" diameter Z ball
> screw and nut at about $300 per foot.

http://www.slidesandballscrews.com/r2005-ballscrew-p-129.html?cPath=39_129_133
with a double, zero-backlash nut at £100.

The cheap option is:
http://www.slidesandballscrews.com/sf2005-ballscrew-p-432.html?cPath=39_128_130
with single, some-backlash nuts at £28.

--
atp

[Kirk Wallace]

On Tue, 2010-11-16 at 20:40 +0000, Andy Pugh wrote:
> On 16 November 2010 20:12, Kirk Wallace <***@wallacecompany.com> wrote:
>
> >> Yes, you can buy them by the foot. (at about $15 a foot)
> >
> > Huh? I would guess ground double nut (for preload) 1.00" diameter Z ball
> > screw and nut at about $300 per foot.
>
> http://www.slidesandballscrews.com/r2005-ballscrew-p-129.html?cPath=39_129_133
> with a double, zero-backlash nut at £100.
>
> The cheap option is:
> http://www.slidesandballscrews.com/sf2005-ballscrew-p-432.html?cPath=39_128_130
> with single, some-backlash nuts at £28.

That pricing is a little hard to believe, but if you are getting good
results, more power to ya. At four feet 20mm diameter is a tad small,
but in the ball park. C7 is good enough for a router, but I wouldn't
like using it on a precision lathe. It's not so much about the accuracy,
because you can map the error out, but you need the accuracy to get
enough preload to get consistent positioning, but not so much that you
get short screw life.

I've been burned on ball screws, more than once, so I lump ball screw
sales in the same boat as used car sales. These people come as close to
lying about their products as possible, so my current thinking is to
order the best I can possibly afford and hope that it is good enough.
--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[William Baden]

Great stuff Kirk.

I have been working on a little table top Atlas/Craftsman lathe for a couple years now. Only have some ways machined. Ended up milling the ways and taking a stone to them to knock off the burrs. Haven't done much more than that.

Will Baden

> From: ***@wallacecompany.com
> To: emc-***@lists.sourceforge.net
> Date: Tue, 16 Nov 2010 12:12:35 -0800
> Subject: Re: [Emc-users] Using a mill as a lathe, EMC2 implications
>
> On Tue, 2010-11-16 at 18:25 +0000, Andy Pugh wrote:
> ... snip
> > > Are ball screws easy to find? Say, I have a 14x48" lathe.
> >
> > Yes, you can buy them by the foot. (at about $15 a foot)
> >
>
> Huh? I would guess ground double nut (for preload) 1.00" diameter Z ball
> screw and nut at about $300 per foot. Then you need to add the precision
> angular contact bearings to mount the screw.
>
> This is my version of the project:
> http://www.wallacecompany.com/cnc_lathe/
>
> It has been on the back burner for a few years :(
>
> --
> Kirk Wallace
> http://www.wallacecompany.com/machine_shop/
> http://www.wallacecompany.com/E45/index.html
> California, USA
>
>
> ------------------------------------------------------------------------------
> Beautiful is writing same markup. Internet Explorer 9 supports
> standards for HTML5, CSS3, SVG 1.1, ECMAScript5, and DOM L2 & L3.
> Spend less time writing and rewriting code and more time creating great
> experiences on the web. Be a part of the beta today
> http://p.sf.net/sfu/msIE9-sfdev2dev
> _______________________________________________
> Emc-users mailing list
> Emc-***@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users

[Jon Elson]

Igor Chudov wrote:
> So, Andy, what is involved? Changing leadscrews to ball screws and
> adding servos etc?
>
> Are ball screws easy to find? Say, I have a 14x48" lathe.
>
Also, you need some scheme to attach an encoder to the spindle.
Depending on the
layout of the headstock, it may be easy or not. Certainly it should be
easier than adding
an encoder to a 1J Bridgeport head, however.

If you want to keep manual operation, then you need a way to disengage
the Z leadscrew,
at the least. As long as the X motor can be made to coast, then that
could just be left connected
all the time. But, if you have a ballscrew on the X, you can't let go
of the handwheel without
locking it in some manner.

Jon

[Jon Elson]

Andy Pugh wrote:
> On 16 November 2010 16:58, Jon Elson <***@pico-systems.com> wrote:
>
>> and I STILL have not gotten around to CNC-ing my lathe.
> Also, threading suddenly becomes trivial. And you can do things like
> to 15.75mm x 0.6mm thread that I used to hold parts of my drawbar
> together, because CNC doesn't care what changewheels you have.
>
Metric threading and tapers are the main reason I would like to CNC it.
It is a totally
massive lathe, came with a DRO, and is amazingly rigid and powerful. On
the same part
I put the ball end on by latheing it in my CNC mill, I used this lathe
to turn a 1" - 20 TPI
thread in 3 passes at 900 RPM. But, it can only do Imperial threads.

Jon

[Andy Pugh]

On 17 November 2010 02:45, Jon Elson <***@pico-systems.com> wrote:

> Metric threading and tapers are the main reason I would like to CNC it.
....
>  But, it can only do Imperial threads.

Assuming it is a conventional lathe with a leadscrew and a power-feed
shaft down the front, then perhaps a solution would be to simply
independently motorise both shafts from the right-hand end?

You would end up with an electronic leadscrew so could cut any pitch,
and the other motor could wind the X out and back in at the ends of
the thread. You would have a lot of backlash, but manual lathes work
perfectly well with backlash so it is probably not a huge issue.

That only really works for threading, unless you use the leadscrew for
all longitudinal feeds. A lot of lathes do work that way (mainly
little ones) so it isn't such a dreadful idea outside of an industrial
context. You would have the option of switching from facing feed to
longitudinal on the "X" motor (interesting from a HAL point of view)

You could still use the lathe manually for your finishing cuts, just
using the CNC for the repetitive cuts, and to cut threads.

--
atp

[Jon Elson]

Andy Pugh wrote:
> Assuming it is a conventional lathe with a leadscrew and a power-feed
> shaft down the front, then perhaps a solution would be to simply
> independently motorise both shafts from the right-hand end?
>
Either way (Acme leadscrew or feed driveshaft), it would have too much
backlash for my liking.
The feeds on this machine are done through metal plate clutches, and I
have no idea of the
cyclic errors in the gear train. If I was going to do it, it would be
done with ballscrews on both
axes.

Jon

[Andy Pugh]

On 17 November 2010 15:30, Jon Elson <***@pico-systems.com> wrote:

> Either way (Acme leadscrew or feed driveshaft), it would have too much
> backlash for my liking.

I have a feeling that backlash is much less of an issue with a lathe
then with a mill, as the cutting forces practically never reverse
during a cut. Trusting to the power feed shaft and apron gearbox for
the X drive might be being a little optimistic though.

--
atp

[Ed]

Andy Pugh wrote:
> On 17 November 2010 15:30, Jon Elson <***@pico-systems.com> wrote:
>
>
>>Either way (Acme leadscrew or feed driveshaft), it would have too much
>>backlash for my liking.
>
>
> I have a feeling that backlash is much less of an issue with a lathe
> then with a mill, as the cutting forces practically never reverse
> during a cut. Trusting to the power feed shaft and apron gearbox for
> the X drive might be being a little optimistic though.
>
Backlash on the X axis gets to be a big problem if you try tapered
threads or any taper that has a reverse force on the tool. The Z axis
usually is not as much of a problem. Ed.

[Igor Chudov]

On Tue, Nov 16, 2010 at 10:58 AM, Jon Elson <***@pico-systems.com> wrote:
> Igor Chudov wrote:
>> The way I think, 180 degrees makes a half ball, and 360 makes a full
>> ball (and would cause it to fall of as you said).
>>
>> So I would like to write code that is capable of cutting more than
>> 180, but less than 360 degrees.
>>
> OK, your description is consistent.  When I think of this, I think in
> the toolpath frame
> of reference, so a 180 degree move is moving the tool 180 degrees around
> the arc.
>>
>> Sounds great. Thanks Jon. This is very exciting, like getting a new machine.
>>
> Yes, it was a quick, slap-dash thing for something I have only rare
> occasion to do,
> and I STILL have not gotten around to CNC-ing my lathe.

Thank you!

I personally would not retrofit a manual lathe, myself.

i

[Jon Elson]

Igor Chudov wrote:
> I personally would not retrofit a manual lathe, myself.
>
Well, I have a rule around here, that I only have one machine of each type.
So, no drill press since I have a vertical mill, and only one lathe. I
do have a
minimill in addition to the Bridgeport, but that is for taking to shows,
mostly.
But, this lathe is such a NICE lathe, that I do have misgivings about
bastardizing it,
even if that bastardizing is entirely reversible. Now that I have a
truly FINE lathe,
it would be REAL hard to go back to a lighter machine. I have MANY
un-fond memories of
trying to do things on an Atlas/Craftsman lathe and having all sorts of
chatter problems, and
am so glad that is a thing of the past.

Jon

[Kirk Wallace]

On Mon, 2010-11-15 at 11:29 -0600, Igor Chudov wrote:
> Andy and Kirk, thanks a lot.
>
> How is Z set up on lathe: does Z increase as I get closer to the lathe chuck?
>
> Anyway, my first project would be to make a round (ball) end to a
> presently square end cylinder. I, obviously, cannot do it in one cut
> due to rigidity. So I would need to make several passes.
>
> Is there a canned cycle or some available subroutine to do so?
>
> Igor

I would tend to use QCAD to draw concentric arcs and other cutter paths,
use dxf2gcode to get the rough code, then test the code with simulated
EMC2 to work out the bugs.

I also have Synergy which will do the all of the path work
automatically, but sometimes it's easier to use QCAD and dxf2gcode,
because I end up having to work out code bugs either way.

You can use g-code o-words to loop the concentric arcs, but I believe
AXIS won't show the looped paths. This isn't essential, but I think
using simple g-code (without the o fluff) is more true to its intent.

I believe axes are supposed to be relative to the workpiece, so you need
to pretend you are sitting on your part as it is spinning. If you see
the cutter moving away from you, then it is moving in a positive
direction.

--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[Andy Pugh]

On 15 November 2010 20:51, Kirk Wallace <***@wallacecompany.com> wrote:

> You can use g-code o-words to loop the concentric arcs, but I believe
> AXIS won't show the looped paths.

It does preview the looped paths.

This might do what you want.

G7
G18
G90.1 ; absolute arc centres
#<rad> = 0.5
#<angle> = 120
#<dia> = 1.5 ; start diameter
#<cut> = 0.10
F2

G0 X0 Z0
G1 X#<dia>
G1 Z [-2 * #<rad>]
G1 X0
#1 = [[#<dia>/2] * 1.3]
O100 WHILE [#1 GT #<rad> + #<cut>]
#1 = [#1 - #<cut>]
G0 Z[#1 - #<rad>]
G0 X0
G3 Z [ #1 * cos[#<angle>] - #<rad>] X [2 * #1 * sin[#<angle>]] I0 K[0-#<rad>]
G1 Z [ #<dia>/2 * cos[#<angle>] - #<rad>] X [#<dia> * sin[#<angle>]]
G0 X [[#<dia>/2] * 3]
O100 END WHILE

#1 = #<rad>
G0 Z 0
G0 X 0
G3 Z [ #1 * cos[#<angle>] - #<rad>] X [2 * #1 * sin[#<angle>]] I0 K[0-#<rad>]
G1 Z [ #<dia>/2 * cos[#<angle>] - #<rad>] X [#<dia> * sin[#<angle>]]
G0 X [#<dia> + 0.2]

M2

--
atp

[Kirk Wallace]

On Mon, 2010-11-15 at 23:05 +0000, Andy Pugh wrote:
> On 15 November 2010 20:51, Kirk Wallace <***@wallacecompany.com> wrote:
>
> > You can use g-code o-words to loop the concentric arcs, but I believe
> > AXIS won't show the looped paths.
>
> It does preview the looped paths.

Oops, you are right, but there is enough other wonkyness that
discourages me from using anything beyond basic g-code. Start form line
doesn't work, you have to figure out what variables you want to restart
from and plug these into your program. Currently my thinking is to do
all the magic in CAM, but I might change my mind at any time.
--
Kirk Wallace
http://www.wallacecompany.com/machine_shop/
http://www.wallacecompany.com/E45/index.html
California, USA

[Jon Elson]

Igor Chudov wrote:
> I have a Bridgeport Interact CNC mill.
>
> Yesterday, I attached a 3 inch lathe chuck to a QC-30 tool holder, so
> I can use this mill as a CNC lathe, without the tailstock of course. I
> would hold the lathe bit in the vise.
>
> Even without a tailstock, I consider this to be a pretty useful
> project,
Yes, I has a need to cut balls on the ends of rods to make custom ball
joints to level a surface plate. I did the sockets with a form tool on
the lathe. But, for the balls, I made an internally threaded collar and
slit it along the axis so it would squeeze the threads when clamped. I
mounted a carbide triangular insert on a QC lathe holder and clamped it
in the vise. I set a few offsets and turned it loose with a simple
program to step inward with am arc move. It made excellent balls,
although it obviously wasn't as rigid as a solid lathe.
> But my question is EMC2 settings and how I can use EMC2 in ways that
> are more lathe specific. Ultimately I want to write a subroutine that
> would change settings to be more lathe-like and another sub that
> changes settings back to more mill-like.
>
> So... what makes a lathe different from a mill? One thing that comes
> to mins is to use XZ plane for circles. That way, I can mill ball ends
> and such, using G2 and G3.
>
Not really much in the motion area is different. Really the only thing
is the tool offsets, and EMC2 now has lathe offsets.
This only matters when you are changing tools in one setup.

Jon