[Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Danny Miller]

I'm managing a community shop with the CNC I designed and built. It's 
running on LinuxCNC 2.7.4


I was told people brought in some Fusion360-generated code that created 
an error "Radius to end arc differs from radius start". Nobody has 
provided me that gcode, so I have no further details. Google saysa this 
was a common issue after a q4 2018 patch to fusion360


People cited this:

https://forums.autodesk.com/t5/fusion-360-computer-aided/help-with-radius-vs-ijk/m-p/7234440#M34397

That the .ini file should assign a new #TOLERANCE_INCH and #TOLERANCE_MM

Does this make sense as a fix?

Danny




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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[jrmitchellj]

I ran into this problem after i botched up a touch-off, and an entry got
into the tool table that should not have been there.
The way to check is to open the tool table in the tool table editor, in the
mode that shows all columns.  If you have offset entries in any column
other than the Z axis, clear them, save & try again.

--J. Ray Mitchell Jr.
jrmitche...@gmail.com



"No problem can be solved from the same level of consciousness that created
it"Albert Einstein


On Sun, Jan 13, 2019 at 10:35 PM Danny Miller  wrote:

> I'm managing a community shop with the CNC I designed and built. It's
> running on LinuxCNC 2.7.4
>
> I was told people brought in some Fusion360-generated code that created
> an error "Radius to end arc differs from radius start". Nobody has
> provided me that gcode, so I have no further details. Google saysa this
> was a common issue after a q4 2018 patch to fusion360
>
> People cited this:
>
>
> https://forums.autodesk.com/t5/fusion-360-computer-aided/help-with-radius-vs-ijk/m-p/7234440#M34397
>
> That the .ini file should assign a new #TOLERANCE_INCH and #TOLERANCE_MM
>
> Does this make sense as a fix?
>
> Danny
>
>
>
>
> ___
> 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] Fusion360 gcode= "Radius to end arc differs from radius start"

[Jon Elson]

On 01/14/2019 12:18 AM, Danny Miller wrote:
I'm managing a community shop with the CNC I designed and 
built. It's running on LinuxCNC 2.7.4


I was told people brought in some Fusion360-generated code 
that created an error "Radius to end arc differs from 
radius start". Nobody has provided me that gcode, so I 
have no further details. Google saysa this was a common 
issue after a q4 2018 patch to fusion360


Yes, a classic problem.  LinuxCNC is strict about the start 
and end radius needing to match to high accuracy.  My fix to 
this is to always use the R word instead of I and J to set 
the arc radius, then there is never any way it can't match.  
If fusion360 cannot be set to use the R word for arc radius, 
then you can try the tolerance adjustment.


Jon


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[dannym]

Is adding a #TOLERANCE_INCH and #TOLERANCE_MM to the .ini file
sufficient?
What tolerances are reasonable?

Danny

-From: "Jon Elson" 
To: "Enhanced Machine Controller (EMC)"
Cc: 
Sent: Monday January 14 2019 10:02:44AM
Subject: Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs
from radius start"

On 01/14/2019 12:18 AM, Danny Miller wrote:
 > I'm managing a community shop with the CNC I designed and 
 > built. It's running on LinuxCNC 2.7.4
 >
 > I was told people brought in some Fusion360-generated code 
 > that created an error "Radius to end arc differs from 
 > radius start". Nobody has provided me that gcode, so I 
 > have no further details. Google saysa this was a common 
 > issue after a q4 2018 patch to fusion360
 >
 Yes, a classic problem. LinuxCNC is strict about the start 
 and end radius needing to match to high accuracy. My fix to 
 this is to always use the R word instead of I and J to set 
 the arc radius, then there is never any way it can't match. 
 If fusion360 cannot be set to use the R word for arc radius, 
 then you can try the tolerance adjustment.

 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] Fusion360 gcode= "Radius to end arc differs from radius start"

[Jon Elson]

On 01/14/2019 10:53 AM, dan...@austin.rr.com wrote:

Is adding a #TOLERANCE_INCH and #TOLERANCE_MM to the .ini file
sufficient?
What tolerances are reasonable?


It depends on how many decimal places your CAM package 
supplies.  If it supplies 4 digits
(X1.2345) then probably .0002 should cover all the roundoff 
errors.


Jon


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[John Figie]

Fusion 360 has a post processor setting to use radius arcs instead of i j
k. Radius arcs is not the default for linuxcnc post. I have been using
Fusion with the default i j k arcs and have had no issues so far.


John Figie

On Mon, Jan 14, 2019, 11:36 AM Jon Elson  On 01/14/2019 10:53 AM, dan...@austin.rr.com wrote:
> > Is adding a #TOLERANCE_INCH and #TOLERANCE_MM to the .ini file
> > sufficient?
> > What tolerances are reasonable?
> >
> >
> It depends on how many decimal places your CAM package
> supplies.  If it supplies 4 digits
> (X1.2345) then probably .0002 should cover all the roundoff
> errors.
>
> 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] Fusion360 gcode= "Radius to end arc differs from radius start"

[John Figie]

I Also want to add that John Elson seems to be saying the opposite of the
LinuxCNC gcode reference. Was that a mistake? Am I missing something?

http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g2-g3

"It is not good practice to program radius format arcs that are nearly full
circles or nearly semicircles because a small change in the location of the
end point will produce a much larger change in the location of the center
of the circle (and, hence, the middle of the arc). The magnification effect
is large enough that rounding error in a number can produce
out-of-tolerance cuts. For instance, a 1% displacement ."

Sincerely,

John Figie

On Tue, Jan 15, 2019, 6:39 AM John Figie  Fusion 360 has a post processor setting to use radius arcs instead of i j
> k. Radius arcs is not the default for linuxcnc post. I have been using
> Fusion with the default i j k arcs and have had no issues so far.
>
>
> John Figie
>
> On Mon, Jan 14, 2019, 11:36 AM Jon Elson 
>> On 01/14/2019 10:53 AM, dan...@austin.rr.com wrote:
>> > Is adding a #TOLERANCE_INCH and #TOLERANCE_MM to the .ini file
>> > sufficient?
>> > What tolerances are reasonable?
>> >
>> >
>> It depends on how many decimal places your CAM package
>> supplies.  If it supplies 4 digits
>> (X1.2345) then probably .0002 should cover all the roundoff
>> errors.
>>
>> 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] Fusion360 gcode= "Radius to end arc differs from radius start"

[andy pugh]

On Tue, 15 Jan 2019 at 19:06, John Figie  wrote:

> "It is not good practice to program radius format arcs that are nearly full
> circles or nearly semicircles because a small change in the location of the
> end point will produce a much larger change in the location of the center
> of the circle

It would be extraordinarily unusual to have a nearly full-circle in
lathe G-code. And even a semicircle is likely to be very unusual.

quarter-circles are very common.

-- 
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


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Stuart Stevenson]

Gentlemen,
  With the R in the G02/G03 program code the control calculates the center
point. When the start point and the end point approach one another any
inaccuracy in either the start point or the end point will cause the center
point calculation to deviate from the desired center point to the extent
the resulting center point location may be out of print tolerance. You will
have the radius accurate as you desire but the location of the radius may
not be where you desire.
  Designating the center point location with the IJK register values will
result in the desired radius center point location. You may be required to
adjust the start position or end position so the control will happily run
your code.
  It is likely you would never see the extreme out of tolerance location
but forewarned is forearmed.
thanks
Stuart


On Tue, Jan 15, 2019 at 1:06 PM John Figie  wrote:

> I Also want to add that John Elson seems to be saying the opposite of the
> LinuxCNC gcode reference. Was that a mistake? Am I missing something?
>
> http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g2-g3
>
> "It is not good practice to program radius format arcs that are nearly full
> circles or nearly semicircles because a small change in the location of the
> end point will produce a much larger change in the location of the center
> of the circle (and, hence, the middle of the arc). The magnification effect
> is large enough that rounding error in a number can produce
> out-of-tolerance cuts. For instance, a 1% displacement ."
>
> Sincerely,
>
> John Figie
>
> On Tue, Jan 15, 2019, 6:39 AM John Figie 
> > Fusion 360 has a post processor setting to use radius arcs instead of i j
> > k. Radius arcs is not the default for linuxcnc post. I have been using
> > Fusion with the default i j k arcs and have had no issues so far.
> >
> >
> > John Figie
> >
> > On Mon, Jan 14, 2019, 11:36 AM Jon Elson  >
> >> On 01/14/2019 10:53 AM, dan...@austin.rr.com wrote:
> >> > Is adding a #TOLERANCE_INCH and #TOLERANCE_MM to the .ini file
> >> > sufficient?
> >> > What tolerances are reasonable?
> >> >
> >> >
> >> It depends on how many decimal places your CAM package
> >> supplies.  If it supplies 4 digits
> >> (X1.2345) then probably .0002 should cover all the roundoff
> >> errors.
> >>
> >> 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
>


-- 
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] Fusion360 gcode= "Radius to end arc differs from radius start"

[Jon Elson]

On 01/15/2019 01:02 PM, John Figie wrote:

I Also want to add that John Elson seems to be saying the opposite of the
LinuxCNC gcode reference. Was that a mistake? Am I missing something?

http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g2-g3

"It is not good practice to program radius format arcs that are nearly full
circles or nearly semicircles because a small change in the location of the
end point will produce a much larger change in the location of the center
of the circle (and, hence, the middle of the arc). The magnification effect
is large enough that rounding error in a number can produce
out-of-tolerance cuts. For instance, a 1% displacement ."


Well, I've been using EMC, EMC2, and LinuxCNC since 1998.  
And, I never program more than 90 degree arcs, so have not 
run into this issue.  It is absolutely true that full 
circles CANNOT be specified with the R form.  I have no idea 
how any particular post processor deals with this problem, 
but it seems likely (since this is NOT a LinuxCNC-specific 
problem, but due to the way the G-code language is 
specified) that a good post would limit R word arcs to 90 
degrees.


I use a bunch of C programs I have written over the years to 
write G-code for specific operations (round holes, slots, 
etc.) and these all use R word arcs in quadrants.


Now that the arc tolerance has been made easily adjustable 
without recompiling source, it is a lot less of an issue.


Jon


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Gene Heskett]

On Tuesday 15 January 2019 22:42:11 Jon Elson wrote:

> On 01/15/2019 01:02 PM, John Figie wrote:
> > I Also want to add that John Elson seems to be saying the opposite
> > of the LinuxCNC gcode reference. Was that a mistake? Am I missing
> > something?
> >
> > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g2-g3
> >
> > "It is not good practice to program radius format arcs that are
> > nearly full circles or nearly semicircles because a small change in
> > the location of the end point will produce a much larger change in
> > the location of the center of the circle (and, hence, the middle of
> > the arc). The magnification effect is large enough that rounding
> > error in a number can produce out-of-tolerance cuts. For instance, a
> > 1% displacement ."
>
> Well, I've been using EMC, EMC2, and LinuxCNC since 1998.
> And, I never program more than 90 degree arcs, so have not
> run into this issue.  It is absolutely true that full
> circles CANNOT be specified with the R form.  I have no idea
> how any particular post processor deals with this problem,
> but it seems likely (since this is NOT a LinuxCNC-specific
> problem, but due to the way the G-code language is
> specified) that a good post would limit R word arcs to 90
> degrees.
>
ISTR doing 75 and 105 degree R word arcs for the corners of a dsub hole 
at some time in the past and had to spec it out to 8 decimal places. But 
since I've learned how to use big johns arcgenm18.py correctly, have 
used only the IJK version much more easily. I often drill a hole by 
using a smaller tool to cut out a plug by setting a depth increment 
of .0075 or so per revolution around the hole going about 10 thou into 
the spoil board.  Slow of course, but I get good holes w/o the drill bit 
grab on the punchthru.
> I use a bunch of C programs I have written over the years to
> write G-code for specific operations (round holes, slots,
> etc.) and these all use R word arcs in quadrants.
>
> Now that the arc tolerance has been made easily adjustable
> without recompiling source, it is a lot less of an issue.

Tell me more about this please.  It is not mentioned in the pdf dox I get 
from master yet.

But in scanning that doc for that, I noted a hal file command that might 
be handy: delf

It sounds as if its a way to remove a setup/test stanza used during the 
machine calibration by removing modules in the addf list after they are 
no longer relevant for normal operation. So since its not mentioned 
anyplace else in the docs, where can I find a discusion/tut on how to 
properly use it?

What I have been doing is just commenting that code out of the file, 
including its addf's.  That may be doing the same thing, saving cycles 
in the loop threads, but I'd like to learn about its proper use.

This getting rid of stuff no longer used would be a lot handier if its 
modules could be included to separate loadrt's, but currently a module 
can only be mentioned in one loadrt, so I am stuck with it in memory 
even if its individual addf is commented out. Then the loadrt's for this 
no longer used stuff could be commented out along with its addf's.

Thanks all.

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 



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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Jon Elson]

On 01/16/2019 01:42 AM, Gene Heskett wrote:

On Tuesday 15 January 2019 22:42:11 Jon Elson wrote:



I use a bunch of C programs I have written over the years to
write G-code for specific operations (round holes, slots,
etc.) and these all use R word arcs in quadrants.


Tell me more about this please.  It is not mentioned in the pdf dox I get
from master yet.



Well, it is NOT part of LinuxCNC.  See :

http://pico-systems.com/gcode.html

for info on some of these.  I really ought to update this 
page with all of my newest programs.
I've added a few more, with ramp-down and a program to cut 
ovals with half-circle round ends to the slots.  There are 
old DOS executables for these, as well as very generic C source.


I have converted one of my programs to Python, and got it to 
give identical output to the C program.  But, I'm not fully 
up to speed on Python, so have not converted the rest, yet.


These do not start the spindle, so you have to edit them all 
manually.  I often stitch together 10 - 30 of these 
individual features to make a complete program, starting the 
spindle at the desired speed in the beginning, and removing 
all M02 lines except the last one.


Jon


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Gene Heskett]

On Wednesday 16 January 2019 11:50:05 Jon Elson wrote:

> On 01/16/2019 01:42 AM, Gene Heskett wrote:
> > On Tuesday 15 January 2019 22:42:11 Jon Elson wrote:
> >> I use a bunch of C programs I have written over the years to
> >> write G-code for specific operations (round holes, slots,
> >> etc.) and these all use R word arcs in quadrants.
> >>
> >>
> >> Tell me more about this please.  It is not mentioned in the pdf dox
> >> I get from master yet.
>
> Well, it is NOT part of LinuxCNC.  See :
>
> http://pico-systems.com/gcode.html
>
> for info on some of these.  I really ought to update this
> page with all of my newest programs.
> I've added a few more, with ramp-down and a program to cut
> ovals with half-circle round ends to the slots.  There are
> old DOS executables for these, as well as very generic C source.
>
> I have converted one of my programs to Python, and got it to
> give identical output to the C program.  But, I'm not fully
> up to speed on Python, so have not converted the rest, yet.
>
> These do not start the spindle, so you have to edit them all
> manually.  I often stitch together 10 - 30 of these
> individual features to make a complete program, starting the
> spindle at the desired speed in the beginning, and removing
> all M02 lines except the last one.
>
> Jon
>
>
Guilty...

> ___
> 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 



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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Gene Heskett]

On Wednesday 16 January 2019 11:50:05 Jon Elson wrote:

> On 01/16/2019 01:42 AM, Gene Heskett wrote:
> > On Tuesday 15 January 2019 22:42:11 Jon Elson wrote:
> >> I use a bunch of C programs I have written over the years to
> >> write G-code for specific operations (round holes, slots,
> >> etc.) and these all use R word arcs in quadrants.
> >>
> >>
> >> Tell me more about this please.  It is not mentioned in the pdf dox
> >> I get from master yet.
>
> Well, it is NOT part of LinuxCNC.  See :
>
> http://pico-systems.com/gcode.html
>
Thread milling looks interesting. Unfortunately I was green as grass when 
I bought a thread mill probably 17 years ago, with an eye to threading 
on the little hf when thats all I had, and the little hf never did grow 
a spindle encoder. But dummy me bought a .750" tool. I could cut OD 
threads with it too, but I don't see it as usefull for internal threads 
w/o at least a 1" hole so it had wiggle room.  So its still in the box & 
never used. As I've never needed to thread that big a hole, and I'd do 
it on the Sheldon now anyway. :) And I did all the threading including 
the long tapers to convert the Sheldon to CNC, did all that on TLM.  Its 
amazing what the tapered gibs did for that $350 lathe.

> for info on some of these.  I really ought to update this
> page with all of my newest programs.
> I've added a few more, with ramp-down and a program to cut
> ovals with half-circle round ends to the slots.  There are
> old DOS executables for these, as well as very generic C source.
>
> I have converted one of my programs to Python, and got it to
> give identical output to the C program.  But, I'm not fully
> up to speed on Python, so have not converted the rest, yet.
>
> These do not start the spindle, so you have to edit them all
> manually.  I often stitch together 10 - 30 of these
> individual features to make a complete program, starting the
> spindle at the desired speed in the beginning, and removing
> all M02 lines except the last one.
>
> Jon
>
>
> ___
> 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 



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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Jon Elson]

On 01/18/2019 09:16 PM, Gene Heskett wrote:
Thread milling looks interesting. Unfortunately I was 
green as grass when I bought a thread mill probably 17 
years ago, with an eye to threading on the little hf when 
thats all I had, and the little hf never did grow a 
spindle encoder.
You don't need a spindle encoder for thread milling.  I have 
used it VERY rarely, but when you decide to make a 
non-standard thread, then it is very handy.  I cut some 
non-standard internal threads on parts at an angle, and it 
made things MUCH easier.  Otherwise, I'd have had to mount a 
vise, spacer blocks and sine bars on a lathe faceplate, 
which sounded like I'd need 5 hands!
So, I put all that on the mill, drilled the starter hole and 
then thread milled it.  Worked like a champ, although slower 
than a lathe would do it.


Jon


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

Re: [Emc-users] Fusion360 gcode= "Radius to end arc differs from radius start"

[Gene Heskett]

On Saturday 19 January 2019 11:37:34 Jon Elson wrote:

> On 01/18/2019 09:16 PM, Gene Heskett wrote:
> > Thread milling looks interesting. Unfortunately I was
> > green as grass when I bought a thread mill probably 17
> > years ago, with an eye to threading on the little hf when
> > thats all I had, and the little hf never did grow a
> > spindle encoder.
>
> You don't need a spindle encoder for thread milling.  I have
> used it VERY rarely, but when you decide to make a
> non-standard thread, then it is very handy.  I cut some
> non-standard internal threads on parts at an angle, and it
> made things MUCH easier.  Otherwise, I'd have had to mount a
> vise, spacer blocks and sine bars on a lathe faceplate,
> which sounded like I'd need 5 hands!
> So, I put all that on the mill, drilled the starter hole and
> then thread milled it.  Worked like a champ, although slower
> than a lathe would do it.
>
> Jon

I've always figured I'd need a 2" 50 tpi adjustable plug & threaded hole 
for something, and use it just to see if I could do it. But so far, 
everything I've needed has been to small to do with a 3/4" OD thread 
mill.  I assume there is a minimum wiggle room in order to get clean 
threads, but I've not seen anything in the #27 book to give a clue how 
much working room it needs before you need to put a few degrees off 
angle for head rotation to get it into some semblance of the same angle 
as the threads ramp equals. But the nut cages for the screws I put in 
the hf were about as big as I've done, no room under those teeny tables 
for anything bigger than about 5/8", somewhat off center because of the 
nuts external return tubes. But the screw turned out to be too short by 
about 2", restricting the x table to about 11" of travel. And that 
eventually was its death nell, even with limit switches, I finally 
screwed it out of the nut, scattering .0635" balls in the debris under 
the table.  And damned if I can find that bag of 500 of those I got from 
ebay all those years ago.

So I bought a 6040 gantry I was trying to bring to life when it got 
rather urgent to get a pacemaker put in, I was down in the mid-thirties 
for a pulse when I decided something was screwing with my balance, 
getting a second or so of dizzyness often enough I was worried about 
falling off a 2 step stepladder. Its working, but I've been told not to 
use my left arm at full extension above my shoulder until the tickle 
wire is well healed (90 days or so, back to warmer weather) into place 
as I might jerk it out of position in my heart! So I'm pretending to 
listen, but I have the missus to care for too. Ever try to tie your 
shoelaces one handed? Or pour water into a Mr. Coffee one handed? I told 
the surgeon when he can teach me how to do that, I'll start wearing the 
sling. I think we have a Mexican standoff. :) In the meantime, I'm not 
picking up anything over 2 lbs with it, or stretching it out at all.

Take care Jon. 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 



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