taper thread on okuma...

[WERNER123]

Hi all.
I`m trying to cut a internal taper thread on a Okuma LC20 osp5000L
here is what my programme looks like.

N540G0X127.631Z9.371
N550G71X133.635Z-88.759H2.0 I-5.794B76.D0.2F6.43M22M32M73

When I run the graphic it runs the taper in the opposite direction.
when I change the "-" to a "+" it comes up with an alarm saying "data word thread cycle"

the book says you can use "I" or "A" so when I use the "A" it goes in the wrong direction again in a "+" value and gives an alarm when I change it to a "-"

I’ve even tried using a "G33" but still not getting it right.

can anyone please help?

[OkumaWiz]

Try to change your X start position to 125 and try again with -I value. I think your "stack up" is getting you.

Best regards,

[littlerob]

Exactly what Wiz said. The H value can be messed with too, but you might end up ripping through your first cut, just give yourself plenty of room, once it's running get it dialed. Basically I start my tool 1 mm below the end of the minor diameter.

[WERNER123]

Thanks guys

I tried dropping the start value to 125 it still came with the same alarm.
I then dropped it to 120 so it cut(on the graphic) but it cuts way under as if 120 was its end point. the angle seems to be right though.
I`ve attached a drawing maybe you can just compare a quick programme...

[WERNER123]

sorry here it is.

[txcncman]

Did you program this with IGF or by hand?

I do not know if this will help you or not:

G71 starts the threading can-cycle

X & Z are end points, X = Finish Root Diameter Z = Z end point

B = the angle of the threading tool (almost always 60)

D = Depth of cut

U = Amount of stock for the last pass

H = Start point (how far above root diameter, should be = to or more than the whole depth of the thread)

I = Taper amount in radius

F = The length that the # of threads are counted in ((F) 1.0”)

J = The thread pitch

M32 = Straight in-feed along thread (on left face)

M73 = Thread cutting pattern #1

[WERNER123]

Thanks I got that. What’s confusing me is the "I" they say it’s the taper amount in radius. So, if my taper is 3deg does that mean I have to actually put in I-1.5? which I have tried and it cut but the angle was out. I think the "I" is for the actual drop from your start to end point in X. the way I got this is I took the distance the tool would travel in Z in this case 98.796mm multiply it with the taper angle in imperial form, in this case 3deg is 0.118 then divide it by 2.
98.796 X 0.118 / 2 = 5.828
I double checked this on edgecam and it came out right, unfortunately I have no post for Okuma on it.

I’m doing something horribly wrong somewhere...

[txcncman]

What is the change in radius from the start of the thread to the finish of the thread? That should be your I.

X127.631 - X133.635 = (D)-6.004

(D)-6.004 / 2 = (R)-3.002

I do not know if that it the actual number for your thread. You did not specify what thread you are actually trying to cut.

[broby]

I is the radial amount of change over the length of cut.
if you are using a thread micrometer and trying for a parallel thread measure the pitch diameter at both ends of the thread and divide the difference by 2.
The answer is the value you use for I.
For external threads, if the diameter at the end of the thread is small use a positive I value, negative if it is larger than the start diameter.
However...
If you are trying to cut a tapered thread of a known included angle use the A command.
Where A is half the included angle (I think...! not at work so can not look up the manual!).
This works far better for cutting tapered threads than using I as you do not need to work out the value for I if the length of the thread changes.
Regards
Brian.

[broby]

Here is a scan of the threading page from one of our manuals.
Hope this helps show what I refer to with the "A" command.
You can see that if you require a 6° (Included angle thread) you could program A177 to get the desired angle on an external thread, or A183 for an Internal thread (Getting smaller towards the end of cut).
Regards
Brian.

[WERNER123]

Thanks guys for the replies I really got some useful info that will help in the future.
Regarding my problem... I finally got it sorted.

I had to put in my major dia where the thread starts into the cycle instead of
the minor where the thread ends.

My "I" value however was still more or less the same I-5... And as broby said the "A" also works.

Correct me if I’m wrong but I’m sure on a Fanuc this is the other way around.

The programme now looks like this.

N540G0X100.0Z10.0M8
N550G71X145.376Z-87.0H2.0I-5.763B76.0D0.2F6.43M22M32M73
N560G0X100.0Z10.0

[broby]

Always program the X value as the major diameter at the start of the thread when programming internal threads, and Minor diameter when cutting External threads.
What kind of thread are you trying to cut?
A thread pitch of 6.43mm?? and an included thread angle of 76°?????
Also, keep in mind that should you wish to change the start point of the threading cycle, your I value will need to be recalculated, but if you use A it does not.