Need Help!- 1/4-18 PIPE THREAD

[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]

Originally Posted by 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.

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]

Originally Posted by cnc-king 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]

Originally Posted by 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...

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?