Hemant Tools - Pune Team

HEMANT TOOLS PVT. LTD. - Pune
PLOT NO. BG/SEI/10/5, NEAR PHILIPS,
ABOVE STANDARD MACHINE TOOLS,
BHOSARI , PUNE-411026
Ph No-020-27129013/65103482

Email ID – pune@hemanttools.co.in , vp@hemanttools.co.in

1) Ms Shrutica - Office Co-Ordianator. -Ph No-020-27129013/65103482

2) Mr. Shailesh - accounts.pune@hemanttools.co.in - 9225625895

G76 - Thread Turning Programe

G76 Programming Example
The G76 requires two (2) lines to give all the information needed to perform the
cycle. It may seem complicated at first but the information is just a numerical description
of the thread. We’ll start by looking at the first (1st) line of the cycle one (1) address at a
time.
LINE #1
G76 P _1 _ _2 _ _ 3_ Q _____ R _____
P has six (6) digits. They are used in three (3) groups of two (2) digits each. The
first group marked #1 indicates the number of finish pass you want to take. All of the
finish stock is taken on the first pass and the remaining passes will all be spring passes
(also called dead passes or pressure passes). In order to take one finish pass and two
spring passes the first two digits of address P will be 03.
The second group of three digits is called the thread pull out. This makes the tool
pull out of the thread, at a 45-degree angle, before reaching the programmed end point.
You use this to prevent a sharp groove at the back of the thread. When you have a thread
relief groove already machined on the part you may not need to use this. In that case the
digits will be 00. In order to pull out ½ thread pitch before the end you would make the
digits 05, to pull out a full thread before the number would be 10.
The last group marked 03 is the thread angle designation. It is used to control the
in feed angle as each pass is taken. This feature keeps the force of cut directed on the
leading edge of the insert. The standard angle in the USA is 60 degree so the last two
digits would be 60. Only the following numbers can be used in this cycle. 80, 60, 55, 30,
29 and 00. You can use different numbers with different thread to help eliminate trouble.
One method would be to use the number 55 with a 60-degree thread. This will put most
of the load on the front of the insert but will also put some on the backside for support.
To obtain the following results the address P will be as such. 1 finish pass 1
spring pass, pull out ½ thread before the end of the thread and a standard 60-degree
thread. P will look like this P020560.
The next address is Q, this is the minimum depth of cut that the cycle will take.
The control calculates its passes and reduces the depth for each pass. With out a
minimum you would end up only taking extremely small amount at the bottom of the
thread. Q is a radial amount and is modal. It remains in effect until changed.
The next address, R, is the finish stock to be left for the finish pass to take. This
will allow a consistent amount of stock to be taken during finishing. All of the stock will
be taken with the first pass and all remaining passes will be spring passes.
Lets look at the first line complete with .005” finish stock and .001” minimum
depth of cut.
G76 P020560 Q10 R50;
That is everything that should go on the first line. You need to end the first line
with an EOB to start the second line. The second line will start with the code G76 just
like the first line. You may also notice that most of the addresses are the same as the first
line. Not to worry, the presence of X and Z tell the control that the address is the same
but the meaning is different.
X is the first address that we come to. It designates the finished diameter of the
thread. This would be the minor diameter for an O/D thread and the major diameter for
an I/D thread. You must take into account that the insert will have a radius put on it from
the carbide manufacturer.
Z is the next address and is the finished Z position at the end of the thread. This is
the point farthest from the start point. You must take into account the acceleration and
deceleration of the axis. This means that you must start the thread about one or two
threads in front of the actual start. You must feed past the required end point by ½ to 1
thread.
The P address is the thread height on one side. You can get this information from
the machineries handbook or other such source. This is measured from the major to
minor diameter on one side only.
Q is the depth of cut on the first pass. The control uses this together with P to
determine the total number of passes it will take. The first pass will always be the deepest
because there is the least amount of tool pressure. From the first pass on the depth of cut
will be less and less each consecutive pass.
R is the amount of taper for taper threads. It is taken as a radial measurement and
the direction is critical. The direction is determined by moving from the start point to the
end point. This is only used for taper threads and is zero or completely omitted if not
needed.
F is the thread lead or distance per revolution between each thread. This is
required to cut the proper thread.
All other rules of threading applied to this cycle, they are as follows.
1) You must be in G97 mode
2) You must maintain the same Z start position
3) You must start your tool clear of the part in X and Z
4) You must start the thread at least one to two threads in front of part
5) You must finish at least ½ to 1 thread after your full thread requirement
6) To recut a thread you cannot change spindle speed, Z start position, Z offset or
use a different tool without risk of destroying the thread.
The finished cycle may look like this:
G00 G97 X2.0 Z.2 S500 M03;
G76 P020560 Q10 R50;
G76 X1.4 Z-1.0 P500 Q100 R0 F.1;
G00 X CLEAR Z CLEAR.

Source - Internet

Higbee Cut /Thread - Blunt Cut - Blunt Thread

I will try my best to explain how it is cut.First what you want to acheive is to remove the part of the thread which is usually a small fin on the turned 45 degree angle portion of the part blank up to where it is a full profile 60 degree thread form.To do this you use a grooving tool after you are done with the threading cycle. First off you must calibrate your threading and grooving tools to the face of the part (or zero.This is where an important trick lies hidden. The center or tip of the threading tip has to be calibrated so it is equal to the leading edge of the groove tool and the groove insert must be as wide or wider than the base of the thread form (an 1/8" wide insert will work up to 8 pitch. etc) Lets say you are doing 10 pitch threads 1" thread length. Now with your regular threading cycle when you program your length you will get 1 full inch of thread and your first full thread length will be z-.100" (a starting length to be deburred) Now program your grooving tool(also in the same threading cycle as used to thread with) to a depth of z-.100" and you are starting to get a deburred thread. You will only need a couple of deburring passes to remove the burr (so play with the starting x value). But there is more to explain !! Spindle rpm and the machines rapid traverse rate will determine the amount of angle of ramp on the deburred thread. The machines rapid rate will stay constant so for a squarer ramp run slower rpms and a tapered ramp more rpms. Only one more tip if after calibrating the tools you have to adjust the z length of cut you must offset the z length equally on both tools.

Not an easy operation to describe with just words and no pictures.We normally leave a 45 plus a little bit of the minor diameter to the + side of the start thread but the higbee cut looks WAY better. might be a tricky deal on a manual lathe with no stop mechanism but Looks like cake on cnc. I looked around the shop and found a coupler that shows exactly what it should look like.Now ..... if I can just make this link work!! http://photos.msn.com/myfiles/folderview.aspx?Folder=4gPozhciq6ZTdypEPFXEQi ctJ*RhGuXgXweAIQIykiw%24 (http://photos.msn.com/myfiles/folderview.aspx?Folder=4gPozhciq6ZTdypEPFXEQictJ*R hGuXgXweAIQIykiw%24)
I have found the G32 threading cycle to be perfect for stuff like this. G32 allows you to control the tool anyway you want to under a threading feed. In the manual for my Haas SL-30 the example is a continuous thread that goes from straight to tapered, then back to straight (I'd be interested to see the nut for this screw). With G32 you can change the vary the pitch while threading. I can't think of an application for this, but it might come in handy sometime. We use this cycle all the time for higby ends, and for taking the spring out of long threaded parts. In other words, you can program a thread that moves the tool into the piece at a variable taper rate to compensate for deflection.

Source - Internet.