[Get lucky]

All right I have never had to program a pipe thread before I took a look in the machinist hand book and just got lost. The machine I am going to to put it in is a kia turn with a fanuc OI-TB control and the threading cycle goes a little like this

1/4-20 cycle

N100M01
T0000
(SINGLE POINT THREADING TOOL)
G97S500M3
X.255Z.1T0000
G76P010060
G76X.189Z-1.65P33(I?)Q30F.05
G28U0W0T0000

I know I can add the tapper for the thread with the "I" in the canded cycle but don't quit under stand start and stop points if somebody could help that would be great

thank you
Kyle

[rk176]

download the threading software from stellram its worked well for me in the past. Im sure the R value in the second g76 line is for the angle.Not at work just now so im not %100 sure

[HuFlungDung]

My seat of the pants method: Disclaimer: I don't run Fanuc, so I cannot interpret your G76 exactly.

First, gather some important info about the thread:
Pipe OD = .540
Effective thread length = .40
Pitch diameter at effective length = .503 (book value)
Thread height = .044 (book value)
taper = 3/4" per foot = .0625" rise (diametral X) per inch of Z run

So if you start with the tool .1" in front of the piece, the total Z travel is .500" During this time the tool withdraws .0625 * .500 = .031" in X, and you might have to split this in half to get "I" if it is a radial amount.

Now the pitch diameter (from the book) is the diameter at the half depth of the thread at the big end. So if you used a sharp tool, then the X endpoint will be as far below the book pitch diameter as the pipe OD is above the pitch diameter.
.540 - .503 = .037 * 2 = .074 therefore the X endpoint will be .540 - .074 = 0.466

I always consider this to be an approximation for a first trial cut, because I've always made final adjustments with the tool offset for a thread tool, to get the engagement correct. Or, the X endpoint could also be tweaked up or down if you would rather leave the tool offset alone.

But if you vary the Z length of the threading pass (you decide its not long enough or you didn't start the tool far enough from the end of the part), then recalculate I because the taper's vector component in X is proportional to the Z length.

[cnc-king]

Hope this will help

this uses the small end dia as reference
N46
(TOOL - 46 OFFSET - 46)
(OD THREAD RIGHT INSERT - NONE)
G18
G30 U0. W0.
T4646
G97 S500 M163
G0 X.7246 Z.096
G76 P010060 Q0 R.002
G76 X.433 Z-.54 P444 Q60 R-.0191 F.05556M9
G30 U0. W0.
M165




this uses the large end dia as reference

G76 P010060 Q0 R.002
G76 X.3993 Z-.54 P444 Q60 R-.0191 F.05556

[cam1]

Made up this spreadsheet using data from the machineries handbook. I've turned mall of th thread sizes at the spindle using this data.

regards

[g-codeguy]

Thread ending point figured at center of 16ER 18 NPT insert and L4 dimension from Machinery's Handbook.

Thread 1/4-18 NPT external
T0101S2000M3
X.58Z.3M8
G76P000155Q30
G76X.467Z-.634P444Q150R-.0291F.05556

Changing starting point or ending point will require R to be modified. R=tan(1+47/60)*(start point + end point) unless both points are the same sign, in which case you would subtract them.

Single block G76
X.58Z.3
G76X.467Z-.634I-.0291K.0444D150F.0556A50.

No disrespect to cnc-king, but no idea what material he is cutting at S500. Although Z.096 will probably work ok at S500, you need to start further away at higher RPM. Z.3 isn't too far, and may work better a bit further away. The Z-axis needs some space to accelerate to the correct feedrate.

The 2-block G76 call DOES NOT use the 'I' for taper.

[cnc-king]

Thread ending point figured at center of 16ER 18 NPT insert and L4 dimension from Machinery's Handbook.

Thread 1/4-18 NPT external
T0101S2000M3
X.58Z.3M8
G76P000155Q30
G76X.467Z-.634P444Q150R-.0291F.05556

Changing starting point or ending point will require R to be modified. R=tan(1+47/60)*(start point + end point) unless both points are the same sign, in which case you would subtract them.

Single block G76
X.58Z.3
G76X.467Z-.634I-.0291K.0444D150F.0556A50.

No disrespect to cnc-king, but no idea what material he is cutting at S500. Although Z.096 will probably work ok at S500, you need to start further away at higher RPM. Z.3 isn't too far, and may work better a bit further away. The Z-axis needs some space to accelerate to the correct feedrate.

The 2-block G76 call DOES NOT use the 'I' for taper.

no offense taken gcode, i normally do not worry about rpm when posting but more about format and structure, due to the fact that i do not what the person is cutting, how rigid is their setup, type of tooling, machine etc. i just assume the person asking the questions has to have some idea about rpm etc, or he or she would not be in the position to be setting up a machine and have no idea what they they are doing.

just my 2 cents - our daewoo accelarates just fine at Z.096 from the face of the part.

[g-codeguy]

no offense taken gcode, i normally do not worry about rpm when posting but more about format and structure, due to the fact that i do not what the person is cutting, how rigid is their setup, type of tooling, machine etc. i just assume the person asking the questions has to have some idea about rpm etc, or he or she would not be in the position to be setting up a machine and have no idea what they they are doing.

just my 2 cents - our daewoo accelarates just fine at Z.096 from the face of the part.

Glad you didn't get upset. Wasn't meant to belittle or any other such negativity. Couple things.

1.) I run some parts with the pipe thread on the cut-off side. Threading insert starts at the cut-off position so there is very little space before the threading insert is cutting the part. Less than the .096 you posted. No bad parts yet because of it, but all my reading in the manuals suggests starting further away. We know it isn't 100% necessary, don't we? Provided the machine is a good one. And provide I don't try to thread at S2000.

2.) I thought the same as you about having sufficient knowledge on feeds and speeds to be a programmer until I started reading this and another machining forum. I have since learned that is not true in some cases. Thus I try to make any data I post to be as accurate as possible.

3.) You are correct in that we have no idea what material is being cut, the rigidity of the set-up, style or grade of insert, and on-and-on.

The OP said he had never cut a pipe thread before. This suggests very little experience. At the very least very little threading experience.

I've used inserts from several different suppliers. They all make inserts capable of threading a 1/4 NPT in 316 SS at S2000. I definitely wouldn't want to position my tool at Z.096 at that RPM. I wouldn't go so far as to say the thread wouldn't be good...but why take the chance?

Z.3 is my normal starting position unless I am threading at S3000 or higher.

[chuy]

I got to back-up king on this one. If a guy doesn't know the what rpm he should be cutting at he shouldn't be programming...

[g-codeguy]

I got to back-up king on this one. If a guy doesn't know the what rpm he should be cutting at he shouldn't be programming...

And yet it happens. Does this mean we should ignore their request for help? I don't mind answering the simple questions. Might be the only ones I can!

I would have liked to know if Lucky was able to thread the part okay. Too often people ask for help, then never let you know if they solved their problem, or got the job running. I'm always curious to know how they made out. Even on the posts I read only, but can't offer help with.

[Get lucky]

well really never got to try my program the plant foreman was hounding me for the part when I had a job that was late in the machine and he told me to go and thread it on the old pipe threader in the corner(didn't know we even had) it work in that sence so no sure if it would have worked but

thank you and everyone for all the help past and presant

Kyle.

[teamus]

I guess I get the x dimension in the execution line ( large od minus pitch dia.) and the r is dependant on the z length but how did you come up with the z length Mr.g code?

[teamus]

all the examples have different x and z dimentions. ???? and the reference to the large and small end the x dimentions are quite different. (cnc king)

[g-codeguy]

First let me say that the X-dimension is NOT large OD minus pitch diameter. Not at work, and I don't have a Machinery's Handbook at home, so I can't give you the exact reason for the final Z-dimension. Sometimes it may be determined by the part drawing itself. The Handbook gives an L1 and L3 dimension. These are sections of the thread length. You have to program a bit further than this or what will happen is the gage for checking the front of the thread reads fine, but the gage for checking the bottom of the thread bottoms out because there isn't enough thread length. This is for an ID pipe thread, of course.

I lay pipe threads out based on the pitch diameter given at the front of an OD thread. This dimension correlates to a fixed distance from the front of an ID thread for each size and is given in the Handbook. I extend this line, offset it 1/2 thread height on both sides, determine how deep I want to thread and draw a vertical line at this depth, analyze X-value of the root at this point, and add the dimension given in the insert catalog from side of insert to insert point. This is my final Z-dimension in the program. I may round it to the nearest .005. Usually will round the X-dimension to the nearest thousandth.

As you can see, the X dimension is based on the tapered root diameter, not the height of the thread. It will change depending on how deep you are threading. This is for the Fanuc controlled lathes we have. Our Okuma is different. It uses the X-value at the tool's starting Z-position instead of the ending position. Naturally this not only changes the sign of the taper, but changes the X-value in the program by a lot from the value you would have in a Fanuc program.

[micktg007]

am having trouble understanding how i program a internal taper thread can somome possably write me a program and this will hopfully help me understand it
the thread is a3/8" bspt X 19tpi and is 5/8 deep would appriciate any help thanks mick

[g-codeguy]

am having trouble understanding how i program a internal taper thread can somome possably write me a program and this will hopfully help me understand it
the thread is a3/8" bspt X 19tpi and is 5/8 deep would appriciate any help thanks mick

You didn't mention what lathe you wanted this program for. I have limited experience as far as the kind of controls. Mostly we have Fanuc controlled lathes, but one Okuma with their control.

Canned cycles.

G76 2-BLOCK CALL

X.54Z.3
G76P000129Q20
G76X.6361Z-.625P337Q90R.0288F.05263

G76 1-BLOCK CALL

X.54Z.3
G76X.6361Z-.625I.0288K.0337D90F.05263A50.

OKUMA

X.54Z.3
G71X.6937Z-.625I-.0288B50D.018U.004H.0674F.05263M32M75

A little explanation:

G76 Q20 denotes minimum DOC (radial) and equals .002
G76 P337 denotes thread height (radial) and equals .0337
G76 P90 is the amount per side of the first pass and equals .009
G76 R.0288 is the taper amount per side over .925 length (.3+.625). Sometimes this number has to be fudged because of tool pressure in order to hold the correct taper.

G71 I-.0288 is the same thing as R in the G76
G71 B50 is the compound infeed angle and does NOT have a decimal
G71 D.018 is the DOC for the first pass and is a diameter value
G71 U.004 is the finish pass allowance and is a diameter value
G71 H.0674 is the thread height and is a diameter value
G71 M32 specifies the cutting mode
G71 M73 specifies the infeed pattern


For the Okuma cycle the X value is taken at Z.3 instead of at Z-.625 as in the G76 cycle. That is why the sign is different for the I value.


G32 cycle

X.54Z.3
G1X.6443F50.
G32X.5867Z-.625F.05263
X.54
G0Z.3
G1X.6563F50.
G32X.5987Z-.625F.05263
X.54
G0Z.3
...
...
...
G1X.6937F50.
G32X.6361Z-.625F.05263
X.54
G0Z1.

G32 cycle allows you to use a compound infeed thusly (25 deg. infeed)

X.54Z.3
G1X.6443F50.
G32X.5867Z-.625F.05263
X.54
G0Z.3
G1X.6561Z.2972F50.
G32X.5987Z-.625F.05263
X.54
G0Z.3
...
...
...
G1X.693Z.2886F50.
G32X.6361Z-.625F.05263
X.54
G0Z1.


G92 cycle

X.54Z.3
G92X.5867Z-.625F.05263R.0288
X.6563
X.6623
...
...
...
X.6937
G0Z1.

Can't use compound infeed with G92 cycle.

HTH

EDIT: Hope you didn't need the examples in metric!
EDIT2: Meant to mention that the only British threads I have programmed were BSPP threads. Sure hope my X values are reasonably close.

[micktg007]

thks g codeguy will try it out first thing monday thks again for your help
mick

[billtheradiator]

Hi

hope this help's

with bspt being a 1 in 16 taper I programme from +6. to -10. in z the x movement equals 1. (diametric) and all proportions of that.

Bill

[g-codeguy]

thks g codeguy will try it out first thing monday thks again for your help
mick

How did you make out?