Re: New to the Okuma lathe with a U10l control
this is all that you use to cut the threads it seems way simple compared to what fusion spit out Im assuming that the G0 x1.273z-3.112m8 is this basically you "zero" for this part and could you also break down the G71 line for me as to what those values are for I'm new too the lathe
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
newton11n
Ok I tried this although it did not produce an error it did not cut threads either it basically acted like a turning program
this may be because it cutted only the 1st pass on the thread, thus a single G32 will only go once towards Z-
to cut the thread, you need all G32s, and in each one you may need both x&z
so :
Code:
(01156.MIN)
N10 G50 S2000
N11 G0 X400.
N12 G0 Z400.
(THREAD1)
N13 T020202
N14 M8
N15 G94
N16 G97 S500 M3 M41
N17 G0 X2.8 Z0.1969
N18 G0 Z0.3181
N19 G1 X1.9496 F39.3701
N20 G32 X1.9496 Z-1.2431 F0.0787
N21 X2.065 Z-1.3009 F0.0787
N22 G0 X2.8
N23 Z0.3181
N24 G1 X1.9311 F39.3701
N25 G32 X1.9311 Z-1.2339 F0.0787
N26 X2.065 Z-1.3009 F0.0787
N27 G0 X2.8
N28 Z0.3181
N29 G1 X1.9168 F39.3701
N30 G32 X1.9168 Z-1.2268 F0.0787
N31 X2.065 Z-1.3009 F0.0787
N32 G0 X2.8
N33 Z0.3181
N34 G1 X1.9049 F39.3701
N35 G32 X1.9049 Z-1.2208 F0.0787
N36 X2.065 Z-1.3009 F0.0787
N37 G0 X2.8
N38 Z0.3181
N39 G1 X1.8943 F39.3701
N40 G32 X1.8943 Z-1.2155 F0.0787
N41 X2.065 Z-1.3009 F0.0787
N42 G0 X2.8
N43 Z0.3181
N44 G1 X1.8943 F39.3701
N45 G32 X1.8943 Z-1.2155 F0.0787
N46 X2.065 Z-1.3009 F0.0787
N47 G0 X2.8
N48 Z0.1969
N49 M9
N50 G90 G0 X400. Z400.
N51 M2
also, like mr wizard said, try G33 instead of G32, and all stuff from post #14 :)
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
newton11n
this is all that you use to cut the threads it seems way simple compared to what fusion spit out Im assuming that the G0 x1.273z-3.112m8 is this basically you "zero" for this part and could you also break down the G71 line for me as to what those values are for I'm new too the lathe
yes the x is the dia it is starting at z is where the threads start, b angle of thread, d depth of cut, h first depth of first pass h height of thread, f feed rate.
Re: New to the Okuma lathe with a U10l control
N13 T020202
N14 M8
N15 G94
N16 G97 S500 M3 M41
N17 G0 X2.8 Z0.1969
N18 G0 Z0.3181
N19 G1 X1.9496 F39.3701
N20 G32 X1.9496 Z-1.2431 F0.0787
N21 X2.065 Z-1.3009 F0.0787
N22 G0 X2.8
N23 Z0.3181
N24 G1 X1.9311 F39.3701
N25 G32 X1.9311 Z-1.2339 F0.0787
N26 X2.065 Z-1.3009 F0.0787
N27 G0 X2.8
N28 Z0.3181
N29 G1 X1.9168 F39.3701
N30 G32 X1.9168 Z-1.2268 F0.0787
N31 X2.065 Z-1.3009 F0.0787
N32 G0 X2.8
N33 Z0.3181
N34 G1 X1.9049 F39.3701
N35 G32 X1.9049 Z-1.2208 F0.0787
N36 X2.065 Z-1.3009 F0.0787
N37 G0 X2.8
I have never seen a threading program
that long. canned cycles are not normally that
long. I am not sure what that is??
Re: New to the Okuma lathe with a U10l control
ok looking at your sample program I see your feed is 1/18 is this your thread pitch? if so am I correct in assuming that for a 12 tpi I would use 1/12
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
newton11n
this is all that you use to cut the threads it seems way simple compared to what fusion spit out
hey newton, that cam spit out a code for threading with an infeed patern at 38 degrees :)
this is the way to attack threads with full control
however, i can not say if this works as it should, because also start Z may need shifting, so to achieve a proper infeed pattern
well, even so, each pass is shorter among Z, and this may lead to increased insert life spam :)
but i guess you were looking for a simple way to do it, and G71 may be just ok for you :)
in all cases, G32/G33 will deliver anytime where G71 will fail ... what can i say ? i hope all your threads to work with G71 :)
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
newton11n
ok looking at your sample program I see your feed is 1/18 is this your thread pitch? if so am I correct in assuming that for a 12 tpi I would use 1/12
actually that is your sample :)
take it easy, one step at a time ... all the best !
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
newton11n
ok looking at your sample program I see your feed is 1/18 is this your thread pitch? if so am I correct in assuming that for a 12 tpi I would use 1/12
yes, you are correct.
as for this,
hey deadly kitten-
(in all cases, G32/G33 will deliver anytime where G71 will fail ... what can i say ? i hope all your threads to work with G71 :))
please share with us how it fails, i guess 25 years has not taught me as much. how would a good machine fail at making threads? they are not really hard to make for most of us,
but it must be a up-hill battle for you. you make things way to hard my man. Kindly!
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
skywalker4
you make things way to hard my man
one day i will go into more details about threading codes ...
Quote:
Originally Posted by
skywalker4
please share with us how it fails
here are some cases that i could not handle with G71
... deliver a stable setup for thousands of parts with 0.03 tolerance, reducing the frequency of edge failure
... use some inserts that were pretty pretentious and replacing them would have created ( days ) downtime
... keep the dimensions somewhere near the NO-GO caliber for tight tolerance, thus increasing the life spam of the insert
... eliminate passes from a G71 cycle, thus using my own approach, which leads to time gain
.. chamfering and threading with the thread insert ( some kind of a mix code )
those were cases where an intervention was required, but there is also prediction : at this point i take into consideration insert geometry, and based on its profile deviation compared to the iso profile, i can generate code specific to each thread tolerance class
and fun parts begins when same producer can not deliver same geometrical tolerances for its inserts ... something like last lot worked, newer ones are trash
i was given drawings with extra specification on thread dimensions, and many calibers : go no-go thread, go-no go cilinder, go no-go for the go, go no-go for the no-go, etc
i could have not delivered those parts without knowledge into threading assemblies tolerances ... and i asked for help at a near by tool factory :)
ps : by the way, if you are interested into desynchronization palier, you may check post4 in here : http://www.cnczone.com/forums/okuma/327510-optimal-clearance.html
Re: New to the Okuma lathe with a U10l control
Kitten, I do agree that you're making the G71 way too difficult.
Also, to insinuate that the rest of us do not cut tight tolerance threads in any production environment is pretty insulting to others.
I'm not saying your way doesn't work, but I can guarantee that G71 is more than capable of any threading needed.
Using G71 makes threading programming substantially easier and offers you the ability to do multiple types of infeed cycles my merely changing a couple M codes on the end of the line.
There's no reason whatsoever that a G71 isn't capable of stable manufacturing.
For those not in the know, G71 is a canned cycle that Okuma uses for threads. I've used it for years on every Okuma I've needed to make parts on from 5000L controls to today.
The format is this:
G0 X1.3
G71 X1.1234 Z-2.3456 H[1.3-1.1234] D.01 B60 U.0005 F1/18 M33 M73
G0 X30 Z30
X: target X end point (not quite theoretical minor diameter but that's usually where I start)
Z: target Z end point (will depend on how you touch off your tool)
H: Thread height (where how tall the thread is so it knows where to start taking cuts from)
D: Depth of cut for first cut (all other cuts will be similar/calculations of this number depending on M codes: M33/M73 M34/M74 or whatever you use)
B: thread angle (60 degree thread, B=60 so on)
U: Finish pass allowance for last thread pass
F: feed rate listed as threads per inch because it's easy to see that's an 18TPI thread as opposed to F.0555
(A value is available in case the threads are tapered)
(I value can be used for tapered threads)
(L value for chamfering at end of thread)
(E value for thread lead variation)
(J in case you use a combo of F/J for thread callouts. Useless in metric mostly)
(Q for multi lead threads)
M codes
The book details what the combinations of these do
I've never met any Okuma guy who prefers to use G33 over G71 for any other reason than continuity from Fanuc code to Okuma code.
But whichever floats your boat.
I'm just saying that G71 is no less capable for 99.9% of the work I've seen and I challenge you to show me a part that this is different.
I did do a test once to prove this on an LB machine where my operator swore by G33. I coded it the way he wanted it and it tool longer to cut threads and he had more issues to the point that by the end of the day he said these words in this order:
"Well that didn't work. I guess we'll stick to G71."
Just because you hear hooves doesn't mean it's a zebra every time.
Sometimes, it's just a damn horse.
1 Attachment(s)
Re: New to the Okuma lathe with a U10l control
Quote:
Kitten, I do agree that you're making the G71 way too difficult
i am not making it difficult, i avoid it :)
Quote:
Also, to insinuate that the rest of us do not cut tight tolerance threads in any production environment is pretty insulting to others
teahole ... no, not like this :) i did not said that others can not cut tight tolerances :) i would not say it not even as a joke :)
Quote:
I've never met any Okuma guy who prefers to use G33 over G71 for any other reason than continuity from Fanuc code to Okuma code
well, besides cases that i encounter, i can tell this about others :
... there had been cases where G71 did not work for others, and needed to use G33
...... onestly, i also think this way, because G71 has its own mind, and is easier to generate what you wish with G33 instead of tweaking the G71 :)
....... real case : conic threads
... there are persons that check if G71 and G33 can work one after another, thus their codes deliver identical spirals in space
....... real case : comparing cnc capabilities between different control generations
... there are persons that use G71 in a single-shot mode, just like G33
....... real case : after threading, need to recut cilinder and repeat finish
at this moment only this cases i have remembered :)
obviously, those are not common cases ... but they are not strange, or should i say those are not forced cases, only to put G71 in a bad light :) and also i dont say that G71 could not do it
Quote:
But whichever floats your boat
not quite ... i dont program only to get floating :) is about full control path with shortest programing time that i can deliver :)
Quote:
I challenge you to show me a part that this is different
all i can say is that it started because of some dimensions, briefs and control that i could not understood back then, and at this moment it became predictive ... thus i can compute out-of-charts tolerances, and so on
i will share when it will be ready
Quote:
I did do a test once to prove this on an LB machine where my operator swore by G33
there is an image attached :
... left : can G71 generate code regardless of point positions inside the section ?
... right : can G71 generate infeed evolution as desired ?
G71 uses inner paterns, and sometimes this patterns are a headache :)
this does not mean that the answer to those questions is no ... but a better answer is G33 :)
Re: New to the Okuma lathe with a U10l control
Thanks for the help everyone I was able to make the G71 work in this instance we are only threading really simple pins for this application and I appreciate the help
Re: New to the Okuma lathe with a U10l control
hi newton / G71 delivers in most cases :)
what your CAM delivered is a more versatile approach, that maybe one day you will find it usefull
is good to know what the Okuma control can do :)
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
deadlykitten
hi newton / G71 delivers in most cases :)
what your CAM delivered is a more versatile approach, that maybe one day you will find it usefull
is good to know what the Okuma control can do :)
deadly,
you really need to look at who is asking the question, if someone is new to this, why overload them with all that info.
he was looking for a simple solution.
I happy that you have all that knowledge, but look at the student better.
also i must say when it comes to threads use the "kiss" method is always a good thing.
Re: New to the Okuma lathe with a U10l control
hy walker :) i did not know what this guy was expecting, and my guess was that he needed help with his code
somewhere i felt that mr newtoon had falled into a trap :)
you know : click+save ! whats thaaaat ? it does not work ... help :)
mr Wizard, which is more experienced, also suggested using rapids when positioning & other stuff :)
teahole also showed up ... his presence is rare, but concentrated :)
well, all is good when it ends with G71 :)
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
skywalker4
also i must say when it comes to threads use the "kiss" method is always a good thing
each one with his own kiss
:*
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
deadlykitten
each one with his own kiss
:*
Exactly,
always good to hear from you!
I am dealing with a guy here right that say's what?? all the time.
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
skywalker4
I am dealing with a guy here right that say's what?? all the time.
i am a bit tired to give an answer to that :) i will reply when thunder strikes :)
Re: New to the Okuma lathe with a U10l control
here are some trials :
Code:
6x 260 240 210 160 110 50
5x 285 265 235 185 60
5x 310 290 240 130 60
9x 180 170 160 140 100 100 80 50 50
9x 180 170 160 150 140 100 50 40 40
10x 240 200 160 120 100 80 40 30 30 30
9x 270 210 170 150 100 40 30 30 30
11x 160 150 150 140 120 100 80 40 30 30 30
12x 120 120 120 120 120 120 100 80 40 30 30 30
similar inserts from different producers have significantly different quality for the cutting edge
such things i run and test pas-by-pas, by taking a look at chip aspect
chips must not be burned, and should not remain on the tool
as a result :
... cutting edges last much longer
... thread aspect increases
... number of tool corections reduces
... rpm can be increased
setup becomes more stable at current specs, thus permitting to increase specs
after a high point is reached, increasing specs even more will deliver less quality parts :)
there is a difference between [ any carbide inserts on any lathe ] vs [ quality carbide inserts on Okuma ]
Re: New to the Okuma lathe with a U10l control
Quote:
Originally Posted by
skywalker4
deadly,
you really need to look at who is asking the question, if someone is new to this, why overload them with all that info.
he was looking for a simple solution.
I happy that you have all that knowledge, but look at the student better.
also i must say when it comes to threads use the "kiss" method is always a good thing.
Hello kywalker4,
This Dumbo has been inflicting himself on Practical M for some time now. His apparent knowledge on the surface has been shown to be a profound lack of knowledge in reality. Empty vessels make the most noise.
Regards,
Bill