开云体育

Hi All,
After finishing my ball screw project and building a new adjustable
mount for my spindle index sensor, I thought I'd try cutting a thread.

I wasn't super happy until I compared it to a comercial 1/4- 20 bolt.
I think the Mach2 threads look better!

I used an HSS bit with essentially no radius, 300 RPM, coolant
flowing, light cuts, and I think 30 passes.

The caption says "first thread" but it was really my third attemp.
The first two times I tried Carbide bits and both times snapped the
end off, a small but fatal piece. I think I'll modify the G-code to
step over the right amount so that I'm only cutting on one side of
the thread. The stepover now is 40% of the infeed, which is a guess,
(need to get out a trig book, high school was 50 years ago).

The variation or errant rpm readings I was having were caused by a
couple shiny spots on my pulley. Pulling the sensor back cured that
until I get some flat black at it.

Jerry

Jerry:

Great news. Yours is the first confirmed thread from Mach2. That sounds
very promising indeed.

Thanks for the update, keep up the great work.

Thanks,
Art
www.artofcnc.ca

Jerry,
Threads look good. I'm glad someone is giving this a try.
I'm in the process of converting an old atlas 6" to cnc and threading
is one of the major jobs I want to use it for. Can I ask what you are
using for a spindle sensor?
Thanks,
Mike

--- In mach1mach2cnc@..., "ozzie34231" <Ozzie@c...> wrote:

Hi All,
After finishing my ball screw project and building a new

adjustable

mount for my spindle index sensor, I thought I'd try cutting a

thread.

Jerry:

Your pictures have made me very happy. Its only a start, much more needs to
be done, but you have proven the concept can work (Which I was very worried
about, buffered pulse threading was a stretch at best...). I only now had
the chance to see the photo's and I must say, they exceed my expectations
for single pulse threading. Hopefully others will find results to be
similar.

Thanks again for your efforts.
Art
www.artofcnc.ca

Maybe a few things made this less than a perfect test:
The extrenely light cuts kept the machine going at a constant speed,
within a couple RPM.
Even with this light cut, there was some chatter, which I couldn,t
hear but I can see on the photo. I need to read up on tool shape and
height for threading.
On the other hand there was some runout as I didn't take time to do a
truing pass before cutting.
I'm not sure the speed was right. The piece is 5/8" diameter and I
cut at 300 rpm with coolant, is that about right Steve?

Certainly I'm happy with it, and it's a start for more rigorous
tests, like taking a cut that does slow the machine.

May I ask the more experienced, what size cuts would you take cutting
20 threads per inch on a non-cnc machine?

Jerry




--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Jerry:

Your pictures have made me very happy. Its only a start, much more

needs to

be done, but you have proven the concept can work (Which I was very

worried

about, buffered pulse threading was a stretch at best...). I only

now had

the chance to see the photo's and I must say, they exceed my

expectations

for single pulse threading. Hopefully others will find results to be
similar.

Thanks again for your efforts.
Art
www.artofcnc.ca

On Tue, 12 Aug 2003 12:51:49 -0000, you wrote:

Maybe a few things made this less than a perfect test:
The extrenely light cuts kept the machine going at a constant speed,
within a couple RPM.
Even with this light cut, there was some chatter, which I couldn,t
hear but I can see on the photo. I need to read up on tool shape and
height for threading.
On the other hand there was some runout as I didn't take time to do a
truing pass before cutting.
I'm not sure the speed was right. The piece is 5/8" diameter and I
cut at 300 rpm with coolant, is that about right Steve?

A little bit slow maybe, for a 1/2"x20 UNF my old post processor would
have done it at 500rpm, with 3 passes at 10 thou, one at 4 thou and
one spring pass. (Total thread depth of 34thou)

That's with an insert, I have 10 thou set as max depth cut for
threading so it works it out itself.

Certainly I'm happy with it, and it's a start for more rigorous
tests, like taking a cut that does slow the machine.

May I ask the more experienced, what size cuts would you take cutting
20 threads per inch on a non-cnc machine?

At that diameter I probably wouldn't have run more than 200rpm
manually!

--
Steve Blackmore

Wow

I think I may be a bit out there but I run about 2000 RPM for a
thread that small..

That is only about 325 FPM. That is SLOW for Carbide and you will get
a better finish at that speed. We run the SECO threading inserts and
that is what it calls for.

So the question is will it Thread at the Higher speeds? A crash at
that speed would not be good...

Have a good one.
Brian

Brian,
Before I used the HSS bit, I tried carbide threading inserts and
chipped two of them, the tiniest piece broke off the end. I had to
use a magnifier to see it but I heard when it happened. In your
opinion, would too slow a speed cause that?

Also, is the correct height at dead center, or a smidgeon above.

Jerry

PS The material is drill rod.




--- In mach1mach2cnc@..., "barker806" <barker1@m...>
wrote:

Wow

I think I may be a bit out there but I run about 2000 RPM for a
thread that small..

That is only about 325 FPM. That is SLOW for Carbide and you will

get

a better finish at that speed. We run the SECO threading inserts

and

that is what it calls for.

So the question is will it Thread at the Higher speeds? A crash at
that speed would not be good...

Have a good one.
Brian

I did thread in 3/4 drill rod at 1500 RPM The pitch was 10 so they
were some deep threads ;) I would say yes to the to slow breaking
inserts because the steel will not shear the same at low speed. I
have had many people in my shop go slow and they have had No luck.
The best way I have found is to find the specs and give it a shot.

If you want to see fast check out the SECO Group No. 1 There
recomindation on the low side is 475 FPM and up to 540 FPM for steel.
The insert has to be RIGHT on the CL. the releaf angles are made to
be on the CL. (people with CNC's are lazy with lathe tools) I can
show you how the Mori SL-15M holds the tool if you like to get the CL
right everytime.

Happy threads
Brian

On Tue, 12 Aug 2003 14:30:07 -0000, you wrote:

I think I may be a bit out there but I run about 2000 RPM for a
thread that small..

No your probably right, my old controller would only run at 1100 RPM
and 16ipm, but since I converted it to PC it will now do 2000RPM and
more than 100ipm! If I change the headstock bearings I can get it to
4000 but for my use it's probably not worth it.

I've been playing with the post processor tonight and reconfigured and
it suggested 2000 rpm :)

That is only about 325 FPM. That is SLOW for Carbide and you will get
a better finish at that speed. We run the SECO threading inserts and
that is what it calls for.

So the question is will it Thread at the Higher speeds? A crash at
that speed would not be good...

No I agree and haven't tried it in anger yet, until I've dry run and
seen what Mach2 thinks it's going to do with the toolpath display I'm
holding fire.

--
Steve Blackmore

You didn't say the type of steel you were threading. The drill rod
steels (silversteel)O-1 W-1, are not the easiest to cut threads on
when compared to free machining steels. I think yours looks just
fine, especially for an early effort with a new program.
Bob

--- In mach1mach2cnc@..., "Robert Hansberger"
<rhansberger@c...> wrote:

You didn't say the type of steel you were threading. The drill rod
steels (silversteel)O-1 W-1, are not the easiest to cut threads on
when compared to free machining steels. I think yours looks just
fine, especially for an early effort with a new program.
Bob

I would say the thread Looks GREAT as well!! because I have used AHHA
to thread with and I couldn't get the spindle speed where it had to
be to get the best finish. If mach2 can do threads fast that would be
nice for all the people doing the small parts.

I am in hopes of setting up a toolroom lathe with Mach2 in the next 6
months for my small work.

Sorry if it sounded like I was putting down the thread because I
understand the hours of work that has been put into those threads.
And I think it is GREAT that there is going to be something that will
work well for threading that will not cost thousands.

Happy chips
Brian

I don't think anybody thought you were putting it down.
Bob

I would say the thread Looks GREAT as well!! because I have used

AHHA

to thread with and I couldn't get the spindle speed where it had to
be to get the best finish. If mach2 can do threads fast that would

be

nice for all the people doing the small parts.

I am in hopes of setting up a toolroom lathe with Mach2 in the next

6

months for my small work.

Sorry if it sounded like I was putting down the thread because I
understand the hours of work that has been put into those threads.
And I think it is GREAT that there is going to be something that

will

work well for threading that will not cost thousands.

Happy chips
Brian

LatheHeads...

to thread with and I couldn't get the spindle speed where it had to

be to get the best finish

Interesting note here on speed. Early on I was told that flashcut had a
problem with threading above a certain speed, so I tried to design the
compensator to allow any speed. This is, of course, impossible, but I am
interested in any experience in this area. The technique is a little unique.
I use a bresenham algorithm within the main bresenham algorithm to slow down
time if the spindle slows. The design assumes the spindle will not speed up
above the starting RPM during a thread (hopefully a good assumption) so time
simply slows down for the pulser which has already computed the pulse timing
using the original algorithm based on the originating spindle speed
feedback. This time slowing is done useing a time constant derived on each
revolution as the adder to the bresenham. There is no way that one pulse per
rev can do the job in the end I think, but I am interested in how fast
anyone CAN do a thread using this technique.
This algorithm within an algorithm was the only way I could think of to
do this reliably in a buffered pulse engine, the results will be
interesting.

To see your theoretical maximum thread pitch at any speed easily , you need
only set a spindle speed, and then jog back and forth in the Z axis. The
reading of the Velocity/Rev DRO at full speed jog is your maximum threading
pitch in your setup. This, of course, is because your rapid speed as
compared to the spindle speed is your maximum pitch per revolution.You'd
need a fast Z carriage to do 2000RPM threading at any but a very fine pitch.
The engine uses the number of 40us intervals between rotations as the
constant for the algorithm as measured when the G32 is begun. So at 500RPM,
the engine has a count of 3000 intervals per rotation, It can correct pretty
finely at that high a number, but at 2000RPM, the count is only 750 so the
ability to compensate has dropped by almost 75% from the 500RPM mark. This
is all at 25Khz. At 45Khz you have 22us periods so the numbers get better.
At 500RPM you get 5454 pulses per rev and at 2000RPM you get 1363 pulses per
revolution. So the quality at 500RPM in 25Khz mode should be equal to the
quality of the cut at 909RPM in 45Khz mode. So just in case you were
wondering if 45Khz mode was any better even if you can't drive your motors
faster, in this case it is because the thread compensation will be more
accurate even at lower speeds.

Just an application note on threading...
Art
www.artofcnc.ca

On Wed, 13 Aug 2003 20:55:09 -0300, you wrote:

Interesting note here on speed. Early on I was told that flashcut had a
problem with threading above a certain speed, so I tried to design the
compensator to allow any speed. This is, of course, impossible, but I am
interested in any experience in this area. The technique is a little unique.
I use a bresenham algorithm within the main bresenham algorithm to slow down
time if the spindle slows. The design assumes the spindle will not speed up
above the starting RPM during a thread (hopefully a good assumption) so time
simply slows down for the pulser which has already computed the pulse timing
using the original algorithm based on the originating spindle speed
feedback. This time slowing is done useing a time constant derived on each
revolution as the adder to the bresenham. There is no way that one pulse per
rev can do the job in the end I think, but I am interested in how fast
anyone CAN do a thread using this technique.

The old controller was quite happy to thread all the pitches I tried
at between 500-800 rpm, with it's limits of 1100rpm top speed, and max
400mm/min axis speed I thought it was pretty good. It was remarkably
accurate too with only one pulse per rev.

I think the limitations in this case were down to a 2Mhz processor and
OS, rather than lathe hardware.

This algorithm within an algorithm was the only way I could think of to
do this reliably in a buffered pulse engine, the results will be
interesting.

How is your basic? That's what the old program was written in <G>. If
you understand it, it may be worth a look to see how it was done?

I think I can retrieve it off the 5 1/4" floppies (If the drive I have
still works).

To see your theoretical maximum thread pitch at any speed easily , you need
only set a spindle speed, and then jog back and forth in the Z axis.

I'll have a play tomorrow and report back.
--
Steve Blackmore

Hi All,
At 2000 RPM cutting 20 threads per inch, my Z axis would have to move
at 100 IPM, ( I think).
Although my top speed is 180 IPM I wonder what distance it would take
to reach that speed. I think my acceleration is set at 3.5 but I
don't know 3.5 what. Can someone tell me what distance it would take
to reach 100 IPM at that setting?

I assume the deceleration would be the same so that potion of the
thread would be useless, No?

Jerry






--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

LatheHeads...

to thread with and I couldn't get the spindle speed where it

had to

be to get the best finish

Interesting note here on speed. Early on I was told that flashcut

had a

problem with threading above a certain speed, so I tried to design

the

compensator to allow any speed. This is, of course, impossible, but

I am

interested in any experience in this area. The technique is a

little unique.

I use a bresenham algorithm within the main bresenham algorithm to

slow down

time if the spindle slows. The design assumes the spindle will not

speed up

above the starting RPM during a thread (hopefully a good

assumption) so time

simply slows down for the pulser which has already computed the

pulse timing

using the original algorithm based on the originating spindle speed
feedback. This time slowing is done useing a time constant derived

on each

revolution as the adder to the bresenham. There is no way that one

pulse per

rev can do the job in the end I think, but I am interested in how

fast

anyone CAN do a thread using this technique.
This algorithm within an algorithm was the only way I could

think of to

do this reliably in a buffered pulse engine, the results will be
interesting.

To see your theoretical maximum thread pitch at any speed easily ,

you need

only set a spindle speed, and then jog back and forth in the Z

axis. The

reading of the Velocity/Rev DRO at full speed jog is your maximum

threading

pitch in your setup. This, of course, is because your rapid speed as
compared to the spindle speed is your maximum pitch per

revolution.You'd

need a fast Z carriage to do 2000RPM threading at any but a very

fine pitch.

The engine uses the number of 40us intervals between rotations as

the

constant for the algorithm as measured when the G32 is begun. So at

500RPM,

the engine has a count of 3000 intervals per rotation, It can

correct pretty

finely at that high a number, but at 2000RPM, the count is only 750

so the

ability to compensate has dropped by almost 75% from the 500RPM

mark. This

is all at 25Khz. At 45Khz you have 22us periods so the numbers get

better.

At 500RPM you get 5454 pulses per rev and at 2000RPM you get 1363

pulses per

revolution. So the quality at 500RPM in 25Khz mode should be equal

to the

quality of the cut at 909RPM in 45Khz mode. So just in case you were
wondering if 45Khz mode was any better even if you can't drive your

motors

faster, in this case it is because the thread compensation will be

more

accurate even at lower speeds.

Just an application note on threading...
Art
www.artofcnc.ca

Art,

Seems a good assumption for all but tapered threads. Comsider pipe
threads: If cut "backwards" and "upside down" (which is common for
many threads, especially blind types) using constant SFPM, the
spindle will increase in speed as the diameter is decreased...

Just a heads up... (probably can "fix" it with a "Don't do this"<G>)

Ballendo


--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

LatheHeads...

The design assumes the spindle will not speed up

above the starting RPM during a thread (hopefully a good

assumption) so time

Hi Jerry:

The 3.5 would be units/sec/sec in other words in one second it will be
doing 3.5*60 units per minute or 210 units per minute, so it takes about 1/2
second to get to speed of 100..

Art
www.artofcnc.ca

Hi Art,
Thanks, but in the example of running at 2000 rpm with the Z axis
needing to move at 100ipm, it would take only 1/100th of a minute to
cut a one inch long thread. I haven't done any calculus for a long
tome but it seems to me that I'd have to start way before the thread
and the deceleration would still ruin it.

If I'm right what kind of Z axis acceleration would one need to be
able to cut at that speed?

Jerry

--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Hi Jerry:

The 3.5 would be units/sec/sec in other words in one second it

will be

doing 3.5*60 units per minute or 210 units per minute, so it takes

about 1/2

second to get to speed of 100..

Art
www.artofcnc.ca

Jerry:

It would be high for sure. If you use 3.5 as you stated, then the distance
would be something on the order of 1.5 inches I think. I'd need calculus to
figure it out, and my calculus sucks. Trial and error in the air might show
it though.


Art
www.artofcnc.ca