Re: [Emc-users] Thoughts on threads, sizing and measuring.

[Gregg Eshelman via Emc-users]

Have the person with the lathe use it to externally thread a length of metal so 
it will screw into something he already has to screw onto the spindle. Then he 
can ship that to you to use for a fit testing piece. 

On Friday, July 31, 2020, 4:26:20 AM MDT, stjohn gold 
 wrote:  
 Hi Andy,
great post, thanks! It all goes to show that threads are complicated. Some
of those standards were written over a period of 20 years, that is no joke.
Nothing to physically test your fit against - brave!

cheers, St.john

On Thu, Jul 30, 2020 at 9:54 PM andy pugh  wrote:

> (Or "Why do I always take 4 goes at a fit with G76")
>
> I recently had the occasion to think harder than normal about threads,
> and especially about their sizing and fits.
> Threads were one of the very first things to be standardised and made
> interchangeable, largely through the work of Josiah Whitworth. And it
> turns out that they are one of the more complicated things to
> standardise.
> The reason I was thinking about this was that I was trying to make a
> lathe faceplate for someone a few hundred miles away. I know that his
> spindle nose is 2 1/4" BSF. (ie, one of Whitworth's threads) but have
> nothing to use for a trial fit.  
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Default Path Blending

[Thaddeus Waldner]

F-engrave might just fit the bill for simple sign work like this. Thanks for 
the info.

> On Jul 31, 2020, at 4:20 PM, Greg Bernard  wrote:
> 
> Have you looked at F-engrave? It's an engraving and V-carving app for
> Linux. scorchworks.com.
> 
> On Fri, Jul 31, 2020, 8:08 AM Thaddeus Waldner  wrote:
> 
>> I’m using Fusion 360 in a workflow for engraving signs. This starts out as
>> a .dxf file, which I import into a fusion 360 sketch, and then use the
>> trace feature to generate tool paths.
>> 
>> As an aside, if anyone has an idea for a simpler workflow (free, of
>> course) and one that perhaps doesn’t involve Windows, Please suggest it
>> here. I’ve tried DXF2GCODE and although it looks like it does all that I
>> need, but I couldn’t get it to work reliably, as it kept skipping features.
>> 
>> The post processes for EMC—as it’s called in Fusion 360—somehow calls for
>> path blending and I cannot figure out where. Is path blending turned on by
>> default, unless you specify exact mode?
>> 
>> Here’s the preamble as generated by the post:
>> 
>> %
>> (ONOFFSWITCHESENGRAVE)
>> (T1  D=0.25 CR=0. TAPER=30DEG - ZMIN=0. - CHAMFER MILL)
>> N10 G90 G94 G17 G91.1
>> N15 G20
>> N20 G53 G0 Z0.
>> (TRACE2)
>> N25 T1 M6
>> N30 S3820 M3
>> N35 G54
>> N40 M8
>> N45 G0 X11.9375 Y0.9635
>> N50 G43 Z0.54 H1
>> N55 G0 Z0.
>> 
>> I was able to fix this by adding the following line:
>> N36 G64 P0.001
>> But I’d like to know how/why it as blending paths in the first place.
>> 
>> 
>> ___
>> 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



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

Re: [Emc-users] Default Path Blending

[Thaddeus Waldner]

Thanks. I’ll take it for a spin.

> On Jul 31, 2020, at 2:53 PM, Bruce Layne  wrote:
> 
> I've been using FreeCAD and I do like it quite a bit.  It's very
> powerful.  The two downsides I see:
> 
> 1) It's currently at version 0.19.  It's not polished software.  It's
> definitely usable as is, but I save my work often.  It does crash
> occasionally, usually when I do something stupid but sometimes for no
> reason that I can discern.
> 
> 2) Like GIMP, the open source user interface isn't the most intuitive. 
> Engraved text in FreeCAD is a good example.  Switch from the Part
> workbench to the Draft workbench.  Select the ShapeString tool.  Enter
> the text, text height and set the path to a TrueType font (it doesn't
> use the system installed fonts).  Switch back to the Part workbench,
> select the shape string that was just created and then select the
> Extrude tool to make it into a 3D object.  You can then make a union of
> the 3D text with another 3D object for raised text, or make a cut of the
> 3D text from another object for engraved text.
> 
> I've been using FreeCAD to put website addresses on the custom parts I'm
> designing that are 3D printed on my MSLA resin 3D printer.  The
> resolution is good enough that a simple font would probably be legible
> in 1mm tall font (not with my old eyes!), although I usually make the
> text 2mm or 3mm tall.
> 
> The above FreeCAD disadvantage #1 is helping with disadvantage #2.  The
> less intuitive user interface features are evolving to be more intuitive
> as the software matures, and that's a good thing.  Unfortunately, it
> introduces a third disadvantage:
> 
> 3) The FreeCAD demo videos on YouTube are quickly obsolete.  Many times,
> I've found a video that explains some feature I want to use in FreeCAD,
> but I'm using a later version of FreeCAD so the demo is fairly useless
> because not only have the buttons all moved, many have disappeared to be
> replaced by different buttons as a more intuitive method is
> implemented.  Overall, it's moving in the right direction but FreeCAD
> still has a few growing pains.
> 
> I'd be a jerk to complain that the completely awesome free open source
> software isn't perfect, and doesn't work exactly the way I think it
> should.  I currently have three different parts that I designed in
> FreeCAD, printing on three different 3D printers.  I've only scratched
> the surface of what FreeCAD can do (finite element analysis, anyone?),
> but I'm definitely a satisfied customer.
> 
> 
> 
> 
> On 7/31/20 3:09 PM, Todd Zuercher wrote:
>> Other free Linux based options might be Inkscape with G-code Tools, or 
>> Freecad.  But both of them might be more painful to learn/use than what 
>> you're doing now.   Of those 2 Freecad is probably the most powerful, but 
>> also the most cumbersome and difficult to use.
> 
> 
> ___
> 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] Default Path Blending

[Thaddeus Waldner]

Yes, for this project I was given the DXF files. 

Aside from that, I haven’t had much luck working with text in Fusion 360. The 
text feature appears to be an afterthought; there is no way to fix alignment of 
text and certain fonts refuse to work altogether. What I’ve been doing is 
designing the artwork in gimp and importing a dxf to a sketch for generating 
the tool path or extruding a solid for 3D printing.



> On Jul 31, 2020, at 2:09 PM, Todd Zuercher  wrote:
> 
> Most likely he is being given artwork from the artist in the form of DXF 
> files that he must turn into machine files that cut out signs.  
> 
> Other free Linux based options might be Inkscape with G-code Tools, or 
> Freecad.  But both of them might be more painful to learn/use than what 
> you're doing now.   Of those 2 Freecad is probably the most powerful, but 
> also the most cumbersome and difficult to use.
> 
> Todd Zuercher
> P. Graham Dunn Inc.
> 630 Henry Street 
> Dalton, Ohio 44618
> Phone:  (330)828-2105ext. 2031
> 
> -Original Message-
> From: Chris Albertson  
> Sent: Friday, July 31, 2020 1:02 PM
> To: Enhanced Machine Controller (EMC) 
> Subject: Re: [Emc-users] Default Path Blending
> 
> [EXTERNAL EMAIL] Be sure links are safe.
> 
> If you want a more simple workflow can't you stay 100% in Fusion360?   I'm
> trying to figure out why you'd need a .dxf file.
> 
> On Fri, Jul 31, 2020 at 6:08 AM Thaddeus Waldner  wrote:
> 
>> I’m using Fusion 360 in a workflow for engraving signs. This starts 
>> out as a .dxf file, which I import into a fusion 360 sketch, and then 
>> use the trace feature to generate tool paths.
>> 
>> As an aside, if anyone has an idea for a simpler workflow (free, of
>> course) and one that perhaps doesn’t involve Windows, Please suggest 
>> it here. I’ve tried DXF2GCODE and although it looks like it does all 
>> that I need, but I couldn’t get it to work reliably, as it kept skipping 
>> features.
>> 
> --
> 
> Chris Albertson
> Redondo Beach, California
> 
> ___
> 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



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

Re: [Emc-users] Thoughts on threads, sizing and measuring.

[andy pugh]

On Fri, 31 Jul 2020 at 23:55, N  wrote:
>
> Have some kind of tool made specifically to measure, bought wrong and never 
> looked close at it.

There are lots of tools. They tend to be expensive and very specific.
For example: https://www.ebay.co.uk/itm/392769109694
Which probably cost over £1000 new, and can only measure 20TPI threads
in a small range around 2".

--
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] Thoughts on threads, sizing and measuring.

[N]

Have some kind of tool made specifically to measure, bought wrong and never 
looked close at it.

> (Or "Why do I always take 4 goes at a fit with G76")
> 
> I recently had the occasion to think harder than normal about threads,
> and especially about their sizing and fits.
> Threads were one of the very first things to be standardised and made
> interchangeable, largely through the work of Josiah Whitworth. And it
> turns out that they are one of the more complicated things to
> standardise.
> The reason I was thinking about this was that I was trying to make a
> lathe faceplate for someone a few hundred miles away. I know that his
> spindle nose is 2 1/4" BSF. (ie, one of Whitworth's threads) but have
> nothing to use for a trial fit.
> 
> Whitworth threads have rounded thread crests and roots. ISO metric has
> flat crests and rounded roots, AN threads had flat roots, but that
> interfered with British rounded crests, so the Unified standard
> emerged which has flat crests and rounded roots.
> 
> For a nut and screw to fit together there needs to be clearance
> between the thread flanks and also clearance between the roots and
> crests of both halves. This means that the roots of the internal
> thread need to be at a larger diameter than the crests of the screw,
> which also means a smaller radius or smaller flat. Similarly the minor
> diameter of the screw needs to be smaller that the through-hole of the
> nut.
> 
> The flank clearance is assured by specifying different "pitch
> diameters" (or "effective diameters") for the internal and external
> threads. The pitch diameter is defined as the line through the thread
> where there is exactly as much air as metal. (ie, where the width of
> the thread is half the pitch.)
> 
> Here is the data for the screw I was making, as an example:
> Size 2 1/4" BSF Internal Thread
> TPI: 6
> Major Dia Min: 2.250
> Effective Dia Min: 2.1570
> Effective Dia Tol: 0.0137
> Effective Dia Min: 2.1433
> Minor Dia Max: 2.0769
> Minor Dia Tol: 0.0403
> Minor Dia Min: 2.0366
> 
> It is interesting that there is no limit to how large the major
> diameter of the internal thread can be. Presumably this means that it
> can be perfectly sharp.
> 
> The "Effective Diameter" is the important measurement when inspecting
> threads, but isn't trivial because it is a measurement of an invisible
> feature.
> 
> There are special thread measuring micrometers with a V anvil and
> point for measuring pitch diameter. And some maths is needed to
> interpret the reading. However each micrometer can only measure 3 or 4
> specific pitches.
> A more accessible way to measure threads is with the "three wire
> method" where three short rods of known diameter are placed in the
> threads. Two on the top in adjacent threads and one at the bottom. The
> measurement over the wires is then taken with a conventional
> micrometer.
> 
> Using this method the pitch diameter can be determined using some
> mathematics, here is an online calculator that I found:
> https://www.cgtk.co.uk/metalwork/calculators/screwmeasurement
> 
> But, 1) I needed to make an internal thread and 2) I needed to make it
> before cutting it. 3) It isn't entirely clear what assumptions such
> calculators are making.
> 
> So, here is another way.
> 
> Firstly, it is possible, but even more fiddly, to measure an internal
> thread using ball bearings and an adjustable parallel. I was measuring
> quite a large thread so could use 3mm balls and a fairly big parallel.
> 
> I drew the required thread in a CAD package, and used tangent circles
> to represent the balls. The pitch diameter in the drawing was set to
> the mid-point of the numbers from the standard.
> 
> I set the thread angle in the drawing to 55 degrees. I probably
> shouldn't have; the perpendicular angle that defines the thread is a
> little larger than the angle along the thread.
> 
> alpha = arctan(P / pi.D). the effective angle is roughly 55 - 1.4 degrees.
> 
> And this turns out to make quite a difference:
> For 55 degrees and a min pitch diameter of 2.1433in the parallel would
> read 49.01mm
> For 53.6 degrees the parallel should read 48.976
> 
> But, the main point of this drawing was _not_ to work out how to
> measure the thread but how to make it.
> 
> The crest radius on the male thread is 0.53mm on this size thread. The
> nut root needs to me smaller. I was using a Seco insert, and so had
> access to the data table, saying that it was a 0.5mm tip radius.
> 
> I then drew the root of the internal thread at this radius, and
> measured the diameter that such an insert would bore at the nominal
> pitch diameter.
> 
> Then at the machine, I used the threading insert to bore its own plain
> hole, and touched it off. I could then use G76 to thread out to the
> major diameter of the thread from the CAD drawing, being fairly
> confident that this would put the pitch diameter where needed.
> 
> In the end it looks like I ended up on the large size, but inside the
> tolerance 

Re: [Emc-users] Thoughts on threads, sizing and measuring.

[andy pugh]

On Fri, 31 Jul 2020 at 22:40, andrew beck  wrote:

> For internal threads I usually use tig wire.  Most machine shops have a tig
> welder and you can bend that and stick it in the bore to measure the
> threads.

I forgot that I had that in the workshop. Though I am not sure that I
have anything big enough for 6 TPI (needs to be about 3mm)

I probably should have written the article more carefully. What I was
really trying to push was the idea of using CAD to do the calcs, and
the modelling of the insert shape in that CAD.

-- 
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] Thoughts on threads, sizing and measuring.

[andrew beck]

That's cool Andy.  I have done similar all the time.  For external threads
I bought a cheap 3wire set that has a chart with it and gives me all the
calculations I need to use.  It's just one simple formula and it tells me
the closest wire size I should be using.

For internal threads I usually use tig wire.  Most machine shops have a tig
welder and you can bend that and stick it in the bore to measure the
threads.

Method 2 is make a test gauge of what size the part should be (eg male part
in your case a dummy lathe spindle.).   Using thread wires to size the
thread.  And then cut the backplate to that size.

Regards

Andrew

On Fri, Jul 31, 2020, 10:26 PM stjohn gold  wrote:

> Hi Andy,
> great post, thanks! It all goes to show that threads are complicated. Some
> of those standards were written over a period of 20 years, that is no joke.
> Nothing to physically test your fit against - brave!
>
> cheers, St.john
>
> On Thu, Jul 30, 2020 at 9:54 PM andy pugh  wrote:
>
> > (Or "Why do I always take 4 goes at a fit with G76")
> >
> > I recently had the occasion to think harder than normal about threads,
> > and especially about their sizing and fits.
> > Threads were one of the very first things to be standardised and made
> > interchangeable, largely through the work of Josiah Whitworth. And it
> > turns out that they are one of the more complicated things to
> > standardise.
> > The reason I was thinking about this was that I was trying to make a
> > lathe faceplate for someone a few hundred miles away. I know that his
> > spindle nose is 2 1/4" BSF. (ie, one of Whitworth's threads) but have
> > nothing to use for a trial fit.
> >
> > Whitworth threads have rounded thread crests and roots. ISO metric has
> > flat crests and rounded roots, AN threads had flat roots, but that
> > interfered with British rounded crests, so the Unified standard
> > emerged which has flat crests and rounded roots.
> >
> > For a nut and screw to fit together there needs to be clearance
> > between the thread flanks and also clearance between the roots and
> > crests of both halves. This means that the roots of the internal
> > thread need to be at a larger diameter than the crests of the screw,
> > which also means a smaller radius or smaller flat. Similarly the minor
> > diameter of the screw needs to be smaller that the through-hole of the
> > nut.
> >
> > The flank clearance is assured by specifying different "pitch
> > diameters" (or "effective diameters") for the internal and external
> > threads. The pitch diameter is defined as the line through the thread
> > where there is exactly as much air as metal. (ie, where the width of
> > the thread is half the pitch.)
> >
> > Here is the data for the screw I was making, as an example:
> > Size 2 1/4" BSF Internal Thread
> > TPI: 6
> > Major Dia Min: 2.250
> > Effective Dia Min: 2.1570
> > Effective Dia Tol: 0.0137
> > Effective Dia Min: 2.1433
> > Minor Dia Max: 2.0769
> > Minor Dia Tol: 0.0403
> > Minor Dia Min: 2.0366
> >
> > It is interesting that there is no limit to how large the major
> > diameter of the internal thread can be. Presumably this means that it
> > can be perfectly sharp.
> >
> > The "Effective Diameter" is the important measurement when inspecting
> > threads, but isn't trivial because it is a measurement of an invisible
> > feature.
> >
> > There are special thread measuring micrometers with a V anvil and
> > point for measuring pitch diameter. And some maths is needed to
> > interpret the reading. However each micrometer can only measure 3 or 4
> > specific pitches.
> > A more accessible way to measure threads is with the "three wire
> > method" where three short rods of known diameter are placed in the
> > threads. Two on the top in adjacent threads and one at the bottom. The
> > measurement over the wires is then taken with a conventional
> > micrometer.
> >
> > Using this method the pitch diameter can be determined using some
> > mathematics, here is an online calculator that I found:
> > https://www.cgtk.co.uk/metalwork/calculators/screwmeasurement
> >
> > But, 1) I needed to make an internal thread and 2) I needed to make it
> > before cutting it. 3) It isn't entirely clear what assumptions such
> > calculators are making.
> >
> > So, here is another way.
> >
> > Firstly, it is possible, but even more fiddly, to measure an internal
> > thread using ball bearings and an adjustable parallel. I was measuring
> > quite a large thread so could use 3mm balls and a fairly big parallel.
> >
> > I drew the required thread in a CAD package, and used tangent circles
> > to represent the balls. The pitch diameter in the drawing was set to
> > the mid-point of the numbers from the standard.
> >
> > I set the thread angle in the drawing to 55 degrees. I probably
> > shouldn't have; the perpendicular angle that defines the thread is a
> > little larger than the angle along the thread.
> >
> > alpha = arctan(P / pi.D). the effective angle is roughly 55 - 1.4
> 

Re: [Emc-users] Default Path Blending

[Greg Bernard]

Have you looked at F-engrave? It's an engraving and V-carving app for
Linux. scorchworks.com.

On Fri, Jul 31, 2020, 8:08 AM Thaddeus Waldner  wrote:

> I’m using Fusion 360 in a workflow for engraving signs. This starts out as
> a .dxf file, which I import into a fusion 360 sketch, and then use the
> trace feature to generate tool paths.
>
> As an aside, if anyone has an idea for a simpler workflow (free, of
> course) and one that perhaps doesn’t involve Windows, Please suggest it
> here. I’ve tried DXF2GCODE and although it looks like it does all that I
> need, but I couldn’t get it to work reliably, as it kept skipping features.
>
> The post processes for EMC—as it’s called in Fusion 360—somehow calls for
> path blending and I cannot figure out where. Is path blending turned on by
> default, unless you specify exact mode?
>
> Here’s the preamble as generated by the post:
>
> %
> (ONOFFSWITCHESENGRAVE)
> (T1  D=0.25 CR=0. TAPER=30DEG - ZMIN=0. - CHAMFER MILL)
> N10 G90 G94 G17 G91.1
> N15 G20
> N20 G53 G0 Z0.
> (TRACE2)
> N25 T1 M6
> N30 S3820 M3
> N35 G54
> N40 M8
> N45 G0 X11.9375 Y0.9635
> N50 G43 Z0.54 H1
> N55 G0 Z0.
>
> I was able to fix this by adding the following line:
> N36 G64 P0.001
> But I’d like to know how/why it as blending paths in the first place.
>
>
> ___
> 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] Default Path Blending

[Bruce Layne]

I've been using FreeCAD and I do like it quite a bit.  It's very
powerful.  The two downsides I see:

1) It's currently at version 0.19.  It's not polished software.  It's
definitely usable as is, but I save my work often.  It does crash
occasionally, usually when I do something stupid but sometimes for no
reason that I can discern.

2) Like GIMP, the open source user interface isn't the most intuitive. 
Engraved text in FreeCAD is a good example.  Switch from the Part
workbench to the Draft workbench.  Select the ShapeString tool.  Enter
the text, text height and set the path to a TrueType font (it doesn't
use the system installed fonts).  Switch back to the Part workbench,
select the shape string that was just created and then select the
Extrude tool to make it into a 3D object.  You can then make a union of
the 3D text with another 3D object for raised text, or make a cut of the
3D text from another object for engraved text.

I've been using FreeCAD to put website addresses on the custom parts I'm
designing that are 3D printed on my MSLA resin 3D printer.  The
resolution is good enough that a simple font would probably be legible
in 1mm tall font (not with my old eyes!), although I usually make the
text 2mm or 3mm tall.

The above FreeCAD disadvantage #1 is helping with disadvantage #2.  The
less intuitive user interface features are evolving to be more intuitive
as the software matures, and that's a good thing.  Unfortunately, it
introduces a third disadvantage:

3) The FreeCAD demo videos on YouTube are quickly obsolete.  Many times,
I've found a video that explains some feature I want to use in FreeCAD,
but I'm using a later version of FreeCAD so the demo is fairly useless
because not only have the buttons all moved, many have disappeared to be
replaced by different buttons as a more intuitive method is
implemented.  Overall, it's moving in the right direction but FreeCAD
still has a few growing pains.

I'd be a jerk to complain that the completely awesome free open source
software isn't perfect, and doesn't work exactly the way I think it
should.  I currently have three different parts that I designed in
FreeCAD, printing on three different 3D printers.  I've only scratched
the surface of what FreeCAD can do (finite element analysis, anyone?),
but I'm definitely a satisfied customer.




On 7/31/20 3:09 PM, Todd Zuercher wrote:
> Other free Linux based options might be Inkscape with G-code Tools, or 
> Freecad.  But both of them might be more painful to learn/use than what 
> you're doing now.   Of those 2 Freecad is probably the most powerful, but 
> also the most cumbersome and difficult to use.


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

Re: [Emc-users] Default Path Blending

[Todd Zuercher]

Most likely he is being given artwork from the artist in the form of DXF files 
that he must turn into machine files that cut out signs.  

Other free Linux based options might be Inkscape with G-code Tools, or Freecad. 
 But both of them might be more painful to learn/use than what you're doing 
now.   Of those 2 Freecad is probably the most powerful, but also the most 
cumbersome and difficult to use.

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

-Original Message-
From: Chris Albertson  
Sent: Friday, July 31, 2020 1:02 PM
To: Enhanced Machine Controller (EMC) 
Subject: Re: [Emc-users] Default Path Blending

[EXTERNAL EMAIL] Be sure links are safe.

If you want a more simple workflow can't you stay 100% in Fusion360?   I'm
trying to figure out why you'd need a .dxf file.

On Fri, Jul 31, 2020 at 6:08 AM Thaddeus Waldner  wrote:

> I’m using Fusion 360 in a workflow for engraving signs. This starts 
> out as a .dxf file, which I import into a fusion 360 sketch, and then 
> use the trace feature to generate tool paths.
>
> As an aside, if anyone has an idea for a simpler workflow (free, of
> course) and one that perhaps doesn’t involve Windows, Please suggest 
> it here. I’ve tried DXF2GCODE and although it looks like it does all 
> that I need, but I couldn’t get it to work reliably, as it kept skipping 
> features.
>
--

Chris Albertson
Redondo Beach, California

___
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] Default Path Blending

[andy pugh]

On Fri, 31 Jul 2020 at 18:15, Matthew Herd  wrote:
>
> I forgot to mention I think there’s a way to alter the startup defaults.

Yes: http://linuxcnc.org/docs/2.8/html/config/ini-config.html#gcode:ini-features
see
RS274NGC_STARTUP_CODE



-- 
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] Default Path Blending

[Matthew Herd]

I forgot to mention I think there’s a way to alter the startup defaults.  
According to the link below, editing "imperial_startup.ngc" can be set to your 
desired parameters, but if you have a reason to change the P value (like using 
a different value for roughing) it won’t return to that value.

See here:  https://forum.linuxcnc.org/plasmac/37612-cut-path-not-following-gcode

> On Jul 31, 2020, at 9:25 AM, Matthew Herd  wrote:
> 
> I just ran into this issue (again).  I did some searching and found that 
> LinuxCNC defaults to G64 with no P value specified as of a certain version 
> (2.7?).  That caused some issues for me over the years, so I’d been manually 
> specifying either G61 (exact path mode) or specifying G64 P0.001 (or another 
> value).  Then recently I’d forgotten to add it and I noticed some drilling 
> cycles were coming dangerously close to breaking the drill off in the part 
> with an X move.  I came across this:
> 
> https://forum.linuxcnc.org/fusion-360/36097-fusion-360-milling-post-with-g64-pn
>  
> 
> 
> I used his post and it seems to generate the necessary values.  I edited the 
> post to default to P0.001.
> 
> Matt
> 
>> On Jul 31, 2020, at 9:05 AM, Thaddeus Waldner > > wrote:
>> 
>> I’m using Fusion 360 in a workflow for engraving signs. This starts out as a 
>> .dxf file, which I import into a fusion 360 sketch, and then use the trace 
>> feature to generate tool paths. 
>> 
>> As an aside, if anyone has an idea for a simpler workflow (free, of course) 
>> and one that perhaps doesn’t involve Windows, Please suggest it here. I’ve 
>> tried DXF2GCODE and although it looks like it does all that I need, but I 
>> couldn’t get it to work reliably, as it kept skipping features.
>> 
>> The post processes for EMC—as it’s called in Fusion 360—somehow calls for 
>> path blending and I cannot figure out where. Is path blending turned on by 
>> default, unless you specify exact mode?
>> 
>> Here’s the preamble as generated by the post:
>> 
>> %
>> (ONOFFSWITCHESENGRAVE)
>> (T1  D=0.25 CR=0. TAPER=30DEG - ZMIN=0. - CHAMFER MILL)
>> N10 G90 G94 G17 G91.1
>> N15 G20
>> N20 G53 G0 Z0.
>> (TRACE2)
>> N25 T1 M6
>> N30 S3820 M3
>> N35 G54
>> N40 M8
>> N45 G0 X11.9375 Y0.9635
>> N50 G43 Z0.54 H1
>> N55 G0 Z0.
>> 
>> I was able to fix this by adding the following line:
>> N36 G64 P0.001
>> But I’d like to know how/why it as blending paths in the first place.
>> 
>> 
>> ___
>> 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] Default Path Blending

[Chris Albertson]

If you want a more simple workflow can't you stay 100% in Fusion360?   I'm
trying to figure out why you'd need a .dxf file.

On Fri, Jul 31, 2020 at 6:08 AM Thaddeus Waldner  wrote:

> I’m using Fusion 360 in a workflow for engraving signs. This starts out as
> a .dxf file, which I import into a fusion 360 sketch, and then use the
> trace feature to generate tool paths.
>
> As an aside, if anyone has an idea for a simpler workflow (free, of
> course) and one that perhaps doesn’t involve Windows, Please suggest it
> here. I’ve tried DXF2GCODE and although it looks like it does all that I
> need, but I couldn’t get it to work reliably, as it kept skipping features.
>
-- 

Chris Albertson
Redondo Beach, California

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

Re: [Emc-users] 7i73 Lagging jog key

[andy pugh]

On Fri, 31 Jul 2020 at 15:15, Peter C. Wallace  wrote:

> Also even with default sserial error management you could only have
> 10 servo thread cycles (10 ms with a 1 ms servo thread) of delay
> due to failed transactions before a sserial error popup would occur.

Maybe noise on the keyboard itself? Is the keycode pin a single clean
transition?

-- 
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] 7i73 Lagging jog key

[Peter C. Wallace]

There does not seem to be any delay in the matrix_kb component:

http://freeby.mesanet.com/matrix_kb.png

Also even with default sserial error management you could only have
10 servo thread cycles (10 ms with a 1 ms servo thread) of delay
due to failed transactions before a sserial error popup would occur.


Peter Wallace
Mesa Electronics


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

Re: [Emc-users] Default Path Blending

[Matthew Herd]

I just ran into this issue (again).  I did some searching and found that 
LinuxCNC defaults to G64 with no P value specified as of a certain version 
(2.7?).  That caused some issues for me over the years, so I’d been manually 
specifying either G61 (exact path mode) or specifying G64 P0.001 (or another 
value).  Then recently I’d forgotten to add it and I noticed some drilling 
cycles were coming dangerously close to breaking the drill off in the part with 
an X move.  I came across this:

https://forum.linuxcnc.org/fusion-360/36097-fusion-360-milling-post-with-g64-pn 


I used his post and it seems to generate the necessary values.  I edited the 
post to default to P0.001.

Matt

> On Jul 31, 2020, at 9:05 AM, Thaddeus Waldner  wrote:
> 
> I’m using Fusion 360 in a workflow for engraving signs. This starts out as a 
> .dxf file, which I import into a fusion 360 sketch, and then use the trace 
> feature to generate tool paths. 
> 
> As an aside, if anyone has an idea for a simpler workflow (free, of course) 
> and one that perhaps doesn’t involve Windows, Please suggest it here. I’ve 
> tried DXF2GCODE and although it looks like it does all that I need, but I 
> couldn’t get it to work reliably, as it kept skipping features.
> 
> The post processes for EMC—as it’s called in Fusion 360—somehow calls for 
> path blending and I cannot figure out where. Is path blending turned on by 
> default, unless you specify exact mode?
> 
> Here’s the preamble as generated by the post:
> 
> %
> (ONOFFSWITCHESENGRAVE)
> (T1  D=0.25 CR=0. TAPER=30DEG - ZMIN=0. - CHAMFER MILL)
> N10 G90 G94 G17 G91.1
> N15 G20
> N20 G53 G0 Z0.
> (TRACE2)
> N25 T1 M6
> N30 S3820 M3
> N35 G54
> N40 M8
> N45 G0 X11.9375 Y0.9635
> N50 G43 Z0.54 H1
> N55 G0 Z0.
> 
> I was able to fix this by adding the following line:
> N36 G64 P0.001
> But I’d like to know how/why it as blending paths in the first place.
> 
> 
> ___
> 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

[Emc-users] Default Path Blending

[Thaddeus Waldner]

I’m using Fusion 360 in a workflow for engraving signs. This starts out as a 
.dxf file, which I import into a fusion 360 sketch, and then use the trace 
feature to generate tool paths. 

As an aside, if anyone has an idea for a simpler workflow (free, of course) and 
one that perhaps doesn’t involve Windows, Please suggest it here. I’ve tried 
DXF2GCODE and although it looks like it does all that I need, but I couldn’t 
get it to work reliably, as it kept skipping features.

The post processes for EMC—as it’s called in Fusion 360—somehow calls for path 
blending and I cannot figure out where. Is path blending turned on by default, 
unless you specify exact mode?

Here’s the preamble as generated by the post:

%
(ONOFFSWITCHESENGRAVE)
(T1  D=0.25 CR=0. TAPER=30DEG - ZMIN=0. - CHAMFER MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(TRACE2)
N25 T1 M6
N30 S3820 M3
N35 G54
N40 M8
N45 G0 X11.9375 Y0.9635
N50 G43 Z0.54 H1
N55 G0 Z0.

I was able to fix this by adding the following line:
N36 G64 P0.001
But I’d like to know how/why it as blending paths in the first place.


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

Re: [Emc-users] Thoughts on threads, sizing and measuring.

[stjohn gold]

Hi Andy,
great post, thanks! It all goes to show that threads are complicated. Some
of those standards were written over a period of 20 years, that is no joke.
Nothing to physically test your fit against - brave!

cheers, St.john

On Thu, Jul 30, 2020 at 9:54 PM andy pugh  wrote:

> (Or "Why do I always take 4 goes at a fit with G76")
>
> I recently had the occasion to think harder than normal about threads,
> and especially about their sizing and fits.
> Threads were one of the very first things to be standardised and made
> interchangeable, largely through the work of Josiah Whitworth. And it
> turns out that they are one of the more complicated things to
> standardise.
> The reason I was thinking about this was that I was trying to make a
> lathe faceplate for someone a few hundred miles away. I know that his
> spindle nose is 2 1/4" BSF. (ie, one of Whitworth's threads) but have
> nothing to use for a trial fit.
>
> Whitworth threads have rounded thread crests and roots. ISO metric has
> flat crests and rounded roots, AN threads had flat roots, but that
> interfered with British rounded crests, so the Unified standard
> emerged which has flat crests and rounded roots.
>
> For a nut and screw to fit together there needs to be clearance
> between the thread flanks and also clearance between the roots and
> crests of both halves. This means that the roots of the internal
> thread need to be at a larger diameter than the crests of the screw,
> which also means a smaller radius or smaller flat. Similarly the minor
> diameter of the screw needs to be smaller that the through-hole of the
> nut.
>
> The flank clearance is assured by specifying different "pitch
> diameters" (or "effective diameters") for the internal and external
> threads. The pitch diameter is defined as the line through the thread
> where there is exactly as much air as metal. (ie, where the width of
> the thread is half the pitch.)
>
> Here is the data for the screw I was making, as an example:
> Size 2 1/4" BSF Internal Thread
> TPI: 6
> Major Dia Min: 2.250
> Effective Dia Min: 2.1570
> Effective Dia Tol: 0.0137
> Effective Dia Min: 2.1433
> Minor Dia Max: 2.0769
> Minor Dia Tol: 0.0403
> Minor Dia Min: 2.0366
>
> It is interesting that there is no limit to how large the major
> diameter of the internal thread can be. Presumably this means that it
> can be perfectly sharp.
>
> The "Effective Diameter" is the important measurement when inspecting
> threads, but isn't trivial because it is a measurement of an invisible
> feature.
>
> There are special thread measuring micrometers with a V anvil and
> point for measuring pitch diameter. And some maths is needed to
> interpret the reading. However each micrometer can only measure 3 or 4
> specific pitches.
> A more accessible way to measure threads is with the "three wire
> method" where three short rods of known diameter are placed in the
> threads. Two on the top in adjacent threads and one at the bottom. The
> measurement over the wires is then taken with a conventional
> micrometer.
>
> Using this method the pitch diameter can be determined using some
> mathematics, here is an online calculator that I found:
> https://www.cgtk.co.uk/metalwork/calculators/screwmeasurement
>
> But, 1) I needed to make an internal thread and 2) I needed to make it
> before cutting it. 3) It isn't entirely clear what assumptions such
> calculators are making.
>
> So, here is another way.
>
> Firstly, it is possible, but even more fiddly, to measure an internal
> thread using ball bearings and an adjustable parallel. I was measuring
> quite a large thread so could use 3mm balls and a fairly big parallel.
>
> I drew the required thread in a CAD package, and used tangent circles
> to represent the balls. The pitch diameter in the drawing was set to
> the mid-point of the numbers from the standard.
>
> I set the thread angle in the drawing to 55 degrees. I probably
> shouldn't have; the perpendicular angle that defines the thread is a
> little larger than the angle along the thread.
>
> alpha = arctan(P / pi.D). the effective angle is roughly 55 - 1.4 degrees.
>
> And this turns out to make quite a difference:
> For 55 degrees and a min pitch diameter of 2.1433in the parallel would
> read 49.01mm
> For 53.6 degrees the parallel should read 48.976
>
> But, the main point of this drawing was _not_ to work out how to
> measure the thread but how to make it.
>
> The crest radius on the male thread is 0.53mm on this size thread. The
> nut root needs to me smaller. I was using a Seco insert, and so had
> access to the data table, saying that it was a 0.5mm tip radius.
>
> I then drew the root of the internal thread at this radius, and
> measured the diameter that such an insert would bore at the nominal
> pitch diameter.
>
> Then at the machine, I used the threading insert to bore its own plain
> hole, and touched it off. I could then use G76 to thread out to the
> major diameter of the thread from the CAD drawing,