[Emc-users] Question on thread geometry

[t***@bgp.nu]

There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.

I want to make a few of these myself and am cutting them using G76 canned cycle on my Emco lathe (I have encoder on spindle, etc) using an Iscar carbide insert 16ER A60 (link below). These are 3/8-24 thread and that falls in the range of the TPI supported by the insert. We have spent time making sure we have the tool lengths, etc dialed in as precisely as possible and are trying to be very careful with our major diameter and thread depth, etc. When measuring the threads we are within specification in terms of pitch diameter and major diameter, etc but the geometry of our thread is very pointy. That is the major diameter peaks are pointy (almost to the point of being sharp) and the root appears to be quite pointy as well, seems to be exactly like the pointy tip of the insert. So, the threads work fine for the purpose but the geometry is bugging me. By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.

I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?

Iscar insert: http://www.iscar.com/eCatalog/item.aspx?cat=5901944&fnum=113&mapp=TH&app=193&GFSTYP=M

-Tom

[Dave Caroline]

As that one has a range then you turn to final diameter ans dont go
too deep with the insert, that leaves a flat on top.
Measure on the job with thread wires etc to check depth.


Dave Caroline

[Marcus Bowman]

If this is a 3/8 x 24 then I assume it is a UNF thread.
As I understand it, UNF (and UNC) threads are part of the UTC system, but the specification for UNF and UNC threads is that UN threads typically have a flat root, with the option of a rounded root. The rounded root simply gives more clearance at the root, so is a benefit, but not a necessary feature. The root could be truncated H/4 from the theoretical vee at the bottom, to give the flat bottom, but the rounding extends beyond that, giving more clearance.
Male UTC threads have a truncated flat top at the peaks, with a width equal to P/8 (or 1/8 of 1/24 of 1 inch, which is about 5 thou in imperial units. The reduction in theoretical OD is twice H/8. H is 0.866025404 x P, so about 72 thou.
Your insert will cut beyond the flat root, so is fine in a normal duty thread. The pitch diameter measurement will guide you as to depth of cut.

UTC threads are metric, but expressed in imperial units, so the A60 insert, which I use myself, is a general purpose insert and may be a compromise between both systems, as well as across the range of pitches the insert can cut accurately. I have had no trouble with fit or finish using the A60 insert (or the A55 insert either).

Marcus

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.
I want to make a few of these myself and am cutting them using G76 canned cycle on my Emco lathe (I have encoder on spindle, etc) using an Iscar carbide insert 16ER A60 (link below). These are 3/8-24 thread and that falls in the range of the TPI supported by the insert. We have spent time making sure we have the tool lengths, etc dialed in as precisely as possible and are trying to be very careful with our major diameter and thread depth, etc. When measuring the threads we are within specification in terms of pitch diameter and major diameter, etc but the geometry of our thread is very pointy. That is the major diameter peaks are pointy (almost to the point of being sharp) and the root appears to be quite pointy as well, seems to be exactly like the pointy tip of the insert. So, the threads work fine for the purpose but the geometry is bugging me. By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.
I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?
Iscar insert: http://www.iscar.com/eCatalog/item.aspx?cat=5901944&fnum=113&mapp=TH&app=193&GFSTYP=M
-Tom
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

[Ken Strauss]

If the proper geometry is important then you may want to consider using full
profile inserts:
http://www.iscar.com/eCatalog/Family.aspx?fnum=126&mapp=TH&app=78&GFSTYP=M

-----Original Message-----
Sent: Friday, June 02, 2017 12:39 PM
To: Enhanced Machine Controller (EMC)
Subject: Re: [Emc-users] Question on thread geometry
If this is a 3/8 x 24 then I assume it is a UNF thread.
As I understand it, UNF (and UNC) threads are part of the UTC system, but

the

specification for UNF and UNC threads is that UN threads typically have a

flat

root, with the option of a rounded root. The rounded root simply gives

more

clearance at the root, so is a benefit, but not a necessary feature. The

root

could be truncated H/4 from the theoretical vee at the bottom, to give the

flat

bottom, but the rounding extends beyond that, giving more clearance.
Male UTC threads have a truncated flat top at the peaks, with a width

equal to

P/8 (or 1/8 of 1/24 of 1 inch, which is about 5 thou in imperial units.

The

reduction in theoretical OD is twice H/8. H is 0.866025404 x P, so about

72

thou.
Your insert will cut beyond the flat root, so is fine in a normal duty

thread. The

pitch diameter measurement will guide you as to depth of cut.
UTC threads are metric, but expressed in imperial units, so the A60

insert,

which I use myself, is a general purpose insert and may be a compromise
between both systems, as well as across the range of pitches the insert

can cut

accurately. I have had no trouble with fit or finish using the A60 insert

(or the

A55 insert either).
Marcus

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get

them the threads have a text-book geometry to them. That is, they have a
small flat top on the major diameter and small flat bottom at the minor
diameter or root. They are made to class 2 or perhaps even class 3. I

know that

these screws I am getting commercially are made using single point carbide
insert tooling on a cnc lathe.

Post by t***@bgp.nu
I want to make a few of these myself and am cutting them using G76

canned

cycle on my Emco lathe (I have encoder on spindle, etc) using an Iscar

carbide

insert 16ER A60 (link below). These are 3/8-24 thread and that falls in

the

range of the TPI supported by the insert. We have spent time making sure

we

have the tool lengths, etc dialed in as precisely as possible and are

trying to be

very careful with our major diameter and thread depth, etc. When

measuring

the threads we are within specification in terms of pitch diameter and

major

diameter, etc but the geometry of our thread is very pointy. That is the

major

diameter peaks are pointy (almost to the point of being sharp) and the

root

appears to be quite pointy as well, seems to be exactly like the pointy

tip of the

insert. So, the threads work fine for the purpose but the geometry is

bugging

me. By the way, this seems to happen for nearly every thread I have cut

on the

machine, but I haven't cared as much in the past as the screws have been

for

my own purposes, but this one will be used in a product sent to customers.

Post by t***@bgp.nu
I am wondering if I am doing something wrong with the insert I am using

or

what. Any thoughts?
http://www.iscar.com/eCatalog/item.aspx?cat=5901944&fnum=113&mapp=T
H&a

Post by t***@bgp.nu
pp=193&GFSTYP=M
-Tom
----------------------------------------------------------------------
-------- Check out the vibrant tech community on one of the world's
most engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

----------------------------------------------------------------------------
--

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

[Ed]

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.
By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.

SNIP

Post by t***@bgp.nu
I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?

Get an insert for that particular TPI, it will leave the proper flat on
the top and bottom of the thread.

Ed.

[t***@bgp.nu]

Ok, thanks for the responses. I found some thread gauge wires and with them have determined that we are cutting too deep. This would cause the pointy peaks and root, so the next question is why are we cutting too deep…? We believe we are entering the correct value for K (thread depth) but I was observing the DRO and Linuxcnc seems to be sending the cutter quite a bit below where it should stop.

I am going to get some more definitive info what is exactly happening, but I am now wondering if there is a bug in the G76 cycle (causing it to cut deeper than it should) or if it is something on my machine…

-Tom

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.
By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.

SNIP

Post by t***@bgp.nu
I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?

Get an insert for that particular TPI, it will leave the proper flat on the top and bottom of the thread.
Ed.
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

[John Kasunich]

How are you touching off (or otherwise determining the X tool offset for the insert)?

For example, if you calculate the offset assuming a sharp-V geometry (the simplest case), but touch off with the actual tip of the insert (not sharp), the insert will be in deeper than LCNC thinks it is when you touch off. So it will cut deeper later.

Post by t***@bgp.nu
Ok, thanks for the responses. I found some thread gauge wires and with them have determined that we are cutting too deep. This would cause the pointy peaks and root, so the next question is why are we cutting too deep…? We believe we are entering the correct value for K (thread depth) but I was observing the DRO and Linuxcnc seems to be sending the cutter quite a bit below where it should stop.
I am going to get some more definitive info what is exactly happening, but I am now wondering if there is a bug in the G76 cycle (causing it to cut deeper than it should) or if it is something on my machine…
-Tom

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.
By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.

SNIP

Post by t***@bgp.nu
I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?

Get an insert for that particular TPI, it will leave the proper flat on the top and bottom of the thread.
Ed.
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

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

[t***@bgp.nu]

To touch the tool off I am physically cutting an OD, measuring that diameter and touching off the tool using that mic’d measurement, so the “actual tip” as you say. So, yes, we are cutting a tiny bit deeper.

However, what we were seeing (and have seen multiple times now but cannot yet re-create at will) is that even though our routine is commanding say, a diameter of .324, the DRO in Axis is showing the cutter down below that. Meaning there is a disconnect between the commanded position and where the machine is really is. The DRO is telling us the truth, if we measure the cut it makes it is indeed where the DRO said it was, but it should never have been cutting that deep. Something very broken is happening periodically (not infrequently) and it seems to be related (but we’re not yet 100% sure) to G76.

We uncovered another (minor? perhaps not related?) bug in the G76 canned cycle. When G76 runs it sets the plane to G17 (we are in G18 on our lathe). In our script we save the modal state before entering, and restore modal state at the end of the routine. We also set G18 inside the routine, but G76 is setting G17 when it runs and the machine stays in G17 after leaving our subroutine. We even tried explicitly setting G18 before exiting our subroutine and it makes no different G76 puts the machine in G17 dammit. That seems like a bug. This is being executed out of Pyngcgui in Axis.

-Tom

Post by John Kasunich
How are you touching off (or otherwise determining the X tool offset for the insert)?
For example, if you calculate the offset assuming a sharp-V geometry (the simplest case), but touch off with the actual tip of the insert (not sharp), the insert will be in deeper than LCNC thinks it is when you touch off. So it will cut deeper later.

Post by t***@bgp.nu
Ok, thanks for the responses. I found some thread gauge wires and with them have determined that we are cutting too deep. This would cause the pointy peaks and root, so the next question is why are we cutting too deep…? We believe we are entering the correct value for K (thread depth) but I was observing the DRO and Linuxcnc seems to be sending the cutter quite a bit below where it should stop.
I am going to get some more definitive info what is exactly happening, but I am now wondering if there is a bug in the G76 cycle (causing it to cut deeper than it should) or if it is something on my machine…
-Tom

Post by t***@bgp.nu
There is a custom adjusting screw that I buy commercially and when I get them the threads have a text-book geometry to them. That is, they have a small flat top on the major diameter and small flat bottom at the minor diameter or root. They are made to class 2 or perhaps even class 3. I know that these screws I am getting commercially are made using single point carbide insert tooling on a cnc lathe.
By the way, this seems to happen for nearly every thread I have cut on the machine, but I haven’t cared as much in the past as the screws have been for my own purposes, but this one will be used in a product sent to customers.

SNIP

Post by t***@bgp.nu
I am wondering if I am doing something wrong with the insert I am using or what. Any thoughts?

Get an insert for that particular TPI, it will leave the proper flat on the top and bottom of the thread.
Ed.
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

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

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

[andy pugh]

Post by t***@bgp.nu
However, what we were seeing (and have seen multiple times now but cannot yet re-create at will) is that even though our routine is commanding say, a diameter of .324, the DRO in Axis is showing the cutter down below that. Meaning there is a disconnect between the commanded position and where the machine is really is.

Are you displaying commanded or actual position? ie, is the axis not
where LinuxCNC commands it to be, or is LinuxCNC not commanding the
numbers from your G76 command?

The G76 code is here:
https://github.com/LinuxCNC/linuxcnc/blob/9e4641a816ab8fe4f6a09a48fac550cc8aef1dee/src/emc/rs274ngc/interp_convert.cc#L4590

That seems quite explicit:
double end_depth = fabs(k_number) + fabs(i_number);

And the last moves are cut at start_x - end_depth

[Gene Heskett]

Post by andy pugh

Post by t***@bgp.nu
However, what we were seeing (and have seen multiple times now but
cannot yet re-create at will) is that even though our routine is
commanding say, a diameter of .324, the DRO in Axis is showing the
cutter down below that. Meaning there is a disconnect between the
commanded position and where the machine is really is.

Are you displaying commanded or actual position? ie, is the axis not
where LinuxCNC commands it to be, or is LinuxCNC not commanding the
numbers from your G76 command?
https://github.com/LinuxCNC/linuxcnc/blob/9e4641a816ab8fe4f6a09a48fac5
50cc8aef1dee/src/emc/rs274ngc/interp_convert.cc#L4590
double end_depth = fabs(k_number) + fabs(i_number);
And the last moves are cut at start_x - end_depth

I've used g76 in odd ways and while the operation was going faster than
the screen DRO updates could track, I haven't been able to touch off at
a known diameter, and cut thread based on the pure math entered. And
sitting here waiting for my coffee to goto work, I am wondering if there
is a g7/g8 interaction thats messing with me? So I commonly start big,
and for externals touch off by small increments until the fit is usable.
That was obviously by small, about 2 thou increments when I was doing the
50 tpi threads in the x drive for the sheldon. 50 tpi because the walls
were thin & I didn't want to weaken it by using a coarser, deeper
thread. It also allowed bearing zero clearance much easier to adjust.
That seems to be holding well as I set it to zero by feel, and the dial
says the backlash is a hair over a thou. I can live with that.

And it sure as tooting beat the nominally 90 thou I started with. The
screw was good, but the nut was a cobbled up mess, had a helicoil insert
in it, running on a square thread screw. And the helicoil was less than
5 thou from being worn and stripped again. I am assuming, never having
asked John Knox if the nuts were available, that one would have to make
his own replacements. Since I had a small ball screw & nut, that was
the obvious choice. I found some oversized balls on ebay, and restuffed
the nuts for nearly zero lash.

What then is the effect of g7/g8 on g76?

Cheers, Gene Heskett

[t***@bgp.nu]

Post by Gene Heskett
What then is the effect of g7/g8 on g76?

Gene,

According to the G76 man page:

"Note:
When G7 Lathe Diameter Mode is in force the values for I, J and K are diameter measurements. When G8 Lathe Radius Mode is in force the values for I, J and K are radius measurements."

Also, according to that page it claims that it is an error if the active plane is not the ZX plane. As I mentioned in a previous email, I set G18 in the script we are running but Linuxcnc/G76 seem hell bent on putting the machine in G17.

-Tom

[Gene Heskett]

Post by t***@bgp.nu

Post by Gene Heskett
What then is the effect of g7/g8 on g76?

Gene,
When G7 Lathe Diameter Mode is in force the values for I, J and K are
diameter measurements. When G8 Lathe Radius Mode is in force the
values for I, J and K are radius measurements."
Also, according to that page it claims that it is an error if the
active plane is not the ZX plane. As I mentioned in a previous email,
I set G18 in the script we are running but Linuxcnc/G76 seem hell bent
on putting the machine in G17.
-Tom

IIRC g17 is xy, perhaps since the joints merge conversion you have a
ghost joint in the configuration? The interactions can be "strange",
although I'll plead to using more "colorfull" words to describe it when
it hits.

TLM is now behaving itself but I did have adjust a few things in that
dept after the joints merge. From its present .ini file:

varname section HEADER:
.ini:JOG_AXES = ZX [DISPLAY]
.ini:GEOMETRY = XZ [DISPLAY]
.ini:COORDINATES = XZ [TRAJ]
.ini:KINEMATICS = trivkins "coordinates=XZ" [KINS]

And:
[RS274NGC]
PARAMETER_FILE = linuxcnc.var
RS274NGC_STARTUP_CODE=G8 G18 G21 G40 G49 G64 P.005 Q.005 G80 G90 G94 G97

best read with a monospaced font.

The reversed order in the first line above "JOG_AXES" is so the jogging
works from the correct keyboard keys both BEFORE and after being homed.

Does this help?

Cheers, Gene Heskett

[t***@bgp.nu]

Post by andy pugh

Post by t***@bgp.nu
However, what we were seeing (and have seen multiple times now but cannot yet re-create at will) is that even though our routine is commanding say, a diameter of .324, the DRO in Axis is showing the cutter down below that. Meaning there is a disconnect between the commanded position and where the machine is really is.

Are you displaying commanded or actual position? ie, is the axis not
where LinuxCNC commands it to be, or is LinuxCNC not commanding the
numbers from your G76 command?

The DRO is showing the actual position. I am pretty sure the commanded position from G76 is being sent correctly, at least when this problem is NOT happening it works fine. I am going to try cutting some more today and will see if I encounter this issue again, though I am not sure what I should look at when it is happening?

Post by andy pugh
https://github.com/LinuxCNC/linuxcnc/blob/9e4641a816ab8fe4f6a09a48fac550cc8aef1dee/src/emc/rs274ngc/interp_convert.cc#L4590
double end_depth = fabs(k_number) + fabs(i_number);
And the last moves are cut at start_x - end_depth

We were talking about looking at the G76 code to see what it was doing, thanks for the pointer to it.

-Tom

Post by andy pugh
--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1916
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

[t***@bgp.nu]

Well, I cut a bunch of screws today, which was executing a repetitive series of gcode routines and I did not have this problem at all. I am now thinking it is caused by something we are doing outside of the G76. We were touching tools off and I am wondering if we did something that caused the discrepancy. It is either that or somehow my steppers lost steps and I didn’t notice it.

I do have a question on thread depth. When entering the theoretical thread depth I always seem cut too shallow (that is, now that I have the tool touched off accurately and am not having the problem with cutting deeper than commanded position). I have to increase the depth a couple thou and re-cut the thread to cut it deep enough. As John Kasunich pointed out it matters how the offset is determined for the tool.

Currently I do that by cutting a diameter with the threading tool. I measure that with a micrometer and I enter the DRO value in the tool touch off for that tool (I have a routine that leaves the tool at the diameter after cutting so this works). But I am wondering, I don’t have a DIAMETER value in the tool table for the tool. Should I? Is a zero (or non-existant) radius value causing Linuxcnc to think the tool is longer than it really is when cutting?

-Tom

Post by andy pugh

Post by t***@bgp.nu
However, what we were seeing (and have seen multiple times now but cannot yet re-create at will) is that even though our routine is commanding say, a diameter of .324, the DRO in Axis is showing the cutter down below that. Meaning there is a disconnect between the commanded position and where the machine is really is.

Are you displaying commanded or actual position? ie, is the axis not
where LinuxCNC commands it to be, or is LinuxCNC not commanding the
numbers from your G76 command?
https://github.com/LinuxCNC/linuxcnc/blob/9e4641a816ab8fe4f6a09a48fac550cc8aef1dee/src/emc/rs274ngc/interp_convert.cc#L4590
double end_depth = fabs(k_number) + fabs(i_number);
And the last moves are cut at start_x - end_depth
--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1916
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

[Jon Elson]

Post by t***@bgp.nu
I have to increase the depth a couple thou and re-cut the thread to cut it deep enough.

Due to machine spring as well as workpiece deflection, a second pass
without even changing the X depth will take off some material. So, if
you turn it down, measure, and then feed in a few thousandths in Z and
cut again and get the desired depth, that will get you a too shallow cut
if you try to cut at the same Z depth on the next part.

Jon

[t***@bgp.nu]

This is a G76 canned cycle and I usually enter 1 (sometimes 2) spring passes. The spring pass(es) take no material so this isn’t a deflection problem.

My theoretical thread depth was 0.0255. I ended up needing to set it to 0.0280, but once set it cuts correctly and repeatably.

I thought it was interesting that 0.0280 - 0.0255 is .0025. .0025 is extremely close the distance between a 0.06mm radius tool and the imaginary tip of that tool ((0.00236 to be precise) ….Coincidence?

-Tom

Post by t***@bgp.nu
I have to increase the depth a couple thou and re-cut the thread to cut it deep enough.

Due to machine spring as well as workpiece deflection, a second pass without even changing the X depth will take off some material. So, if you turn it down, measure, and then feed in a few thousandths in Z and cut again and get the desired depth, that will get you a too shallow cut if you try to cut at the same Z depth on the next part.
Jon
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users

[Jon Elson]

Post by t***@bgp.nu
This is a G76 canned cycle and I usually enter 1 (sometimes 2) spring passes. The spring pass(es) take no material so this isn’t a deflection problem.
My theoretical thread depth was 0.0255. I ended up needing to set it to 0.0280, but once set it cuts correctly and repeatably.
I thought it was interesting that 0.0280 - 0.0255 is .0025. .0025 is extremely close the distance between a 0.06mm radius tool and the imaginary tip of that tool ((0.00236 to be precise) ….Coincidence?

I might not be understanding the geometry. BUT, if you are using
calculations based on a sharply-pointed tool tip, and then touch off a
truncated tool to the material, you will end up with an undersize
external thread. This is because you are zeroing the tool's
thread-cutting flanks too close to the work. So, you have to compensate
for the truncated tool tip. If you want to touch off the tool tip, or
cut and measure a diameter with the tool tip, then set the zero smaller
than the measured work by the amount the tip is truncated (all in radius
measure.)

Jon

[Gene Heskett]

Post by Jon Elson

Post by t***@bgp.nu
I have to increase the depth a couple thou and re-cut the thread
to cut it deep enough.

Due to machine spring as well as workpiece deflection, a second pass
without even changing the X depth will take off some material. So, if
you turn it down, measure, and then feed in a few thousandths in Z and
cut again and get the desired depth, that will get you a too shallow
cut if you try to cut at the same Z depth on the next part.
Jon

This I think is one of the reasons for G76 H parameter, where it makes H
passes at the final depth, often called spring cuts. And I've noted
that since I installed the shop made toolpost holder, replacing the
springy compound, and tapered gibs on TLM, that the ending spring cuts
aren't taking off a cut to speak of during the spring cuts, so machine
rigidity does make a difference. I'll be somewhat surprised if, when I
make my first threads on the sheldon, I see an actual cutting action
after the first H pass. Even w/o tapered gibs, the huge H pattern to
its carriages footprint should be more rigid than TLM's very narrow
carriage footprint with the tapered gibs. But first I need to do the
poor mans set-true on that 3 jaw, its running about 3 thou eccentric. I
think it can do better. If not, I'll have to buy a 4 jaw independant and
big bore backplate.

Cheers, Gene Heskett

[Jon Elson]

Post by Jon Elson

Post by t***@bgp.nu
I have to increase the depth a couple thou and re-cut the thread to cut it deep enough.

Due to machine spring as well as workpiece deflection, a second pass
without even changing the X depth will take off some material. So, if
you turn it down, measure, and then feed in a few thousandths in Z and
cut again and get the desired depth, that will get you a too shallow
cut if you try to cut at the same Z depth on the next part.

All these "Z"s should be "X"s. What I was trying to show was that two
passes of cutting without advancing X can keep reducing the diameter.

Jon

Jon

[andy pugh]

Post by t***@bgp.nu
Currently I do that by cutting a diameter with the threading tool. I
measure that with a micrometer and I enter the DRO value in the tool touch
off for that tool (I have a routine that leaves the tool at the diameter
after cutting so this works). But I am wondering, I don’t have a DIAMETER
value in the tool table for the tool. Should I? Is a zero (or
non-existant) radius value causing Linuxcnc to think the tool is longer
than it really is when cutting?

How do your numbers compare with line 502 of this spreadsheet?
https://docs.google.com/spreadsheets/d/1m5zkO9-SbQaYWbTPlQXJ2VA73Ys8WgWDrPk_rEukHc0/edit?ts=57064122#gid=0

(This is a version of the table I complied 20 years or so ago, but modified
to include the effects of crest and root flattening/rounding)

The DXF file of the inserts shows a 0.05mm radius, whereas as the web-page
table shows 0.06mm. In either case the tip is rounded, not flat.

You might consider drawing the thread in CAD, with the exact profile for
the thread and grade required, and then fit an exact drawing of the insert
into it. That might answer the question of how to touch-off and what to.

It is an interesting puzzle, and I am another who will admit to "creeping
up" on one-off threads.

[Gene Heskett]

Post by andy pugh

Post by t***@bgp.nu
Currently I do that by cutting a diameter with the threading tool.
I measure that with a micrometer and I enter the DRO value in the
tool touch off for that tool (I have a routine that leaves the tool
at the diameter after cutting so this works). But I am wondering, I
don’t have a DIAMETER value in the tool table for the tool. Should
I? Is a zero (or non-existant) radius value causing Linuxcnc to
think the tool is longer than it really is when cutting?

How do your numbers compare with line 502 of this spreadsheet?
https://docs.google.com/spreadsheets/d/1m5zkO9-SbQaYWbTPlQXJ2VA73Ys8Wg
WDrPk_rEukHc0/edit?ts=57064122#gid=0
(This is a version of the table I complied 20 years or so ago, but
modified to include the effects of crest and root flattening/rounding)
The DXF file of the inserts shows a 0.05mm radius, whereas as the
web-page table shows 0.06mm. In either case the tip is rounded, not
flat.
You might consider drawing the thread in CAD, with the exact profile
for the thread and grade required, and then fit an exact drawing of
the insert into it. That might answer the question of how to touch-off
and what to.
It is an interesting puzzle, and I am another who will admit to
"creeping up" on one-off threads.

Even the "creep up" can lead to fit problems. I cannot buy an insert
truely suitable for cutting a 50 TPI thread, all are tip profiled for
much coarser threads, and rarely is the tip profile correct for a thread
3x finer than a 16 to 20 TPI thread. So the nuts I might make for a 50
TPI thread, I expect to have to drive with spanners, well lubed, as
they'll need to round off the sharper tips of each the first time
assembled. Yet 3 trips later, they'll need some thread-locker magic to
stay put. Neither actually has a full bodied width of tooth. Whats
needed is an HSS insert with a sharp tip that might be flattened about
half a red one on a wet rouge stone. Cheap enough to bin when its dull
w/o shedding a tear because the carbide version is so outragiously
priced. The insert makers are not serving the market with what the
market needs.

Cheers, Gene Heskett

[t***@bgp.nu]

My numbers are similar (not exactly the same):

Major Dia: 0.3678
Minor Dia: 0.3239
Thread Depth: 0.2555

I am measuring with thread wires (0.029 dia) and am trying to get a pitch dia of between 0.3468 and .3430 (class 2A or better).

-Tom

Post by andy pugh

Post by t***@bgp.nu
Currently I do that by cutting a diameter with the threading tool. I
measure that with a micrometer and I enter the DRO value in the tool touch
off for that tool (I have a routine that leaves the tool at the diameter
after cutting so this works). But I am wondering, I don’t have a DIAMETER
value in the tool table for the tool. Should I? Is a zero (or
non-existant) radius value causing Linuxcnc to think the tool is longer
than it really is when cutting?

How do your numbers compare with line 502 of this spreadsheet?
https://docs.google.com/spreadsheets/d/1m5zkO9-SbQaYWbTPlQXJ2VA73Ys8WgWDrPk_rEukHc0/edit?ts=57064122#gid=0
(This is a version of the table I complied 20 years or so ago, but modified
to include the effects of crest and root flattening/rounding)
The DXF file of the inserts shows a 0.05mm radius, whereas as the web-page
table shows 0.06mm. In either case the tip is rounded, not flat.
You might consider drawing the thread in CAD, with the exact profile for
the thread and grade required, and then fit an exact drawing of the insert
into it. That might answer the question of how to touch-off and what to.
It is an interesting puzzle, and I am another who will admit to "creeping
up" on one-off threads.
--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is designed
for the especial use of mechanical geniuses, daredevils and lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1916
------------------------------------------------------------------------------
Check out the vibrant tech community on one of the world's most
engaging tech sites, Slashdot.org! http://sdm.link/slashdot
_______________________________________________
Emc-users mailing list
https://lists.sourceforge.net/lists/listinfo/emc-users