1/4 NPT thread mill

[gcode]

We've got about 30 CNC's here and produce thousands of NPT threads a month

ranging from 1/8-27 up to 4" -8

 

We do it all in Mastercam.

 

I use an old Stellram app to get the major diameter of the thread (1.308" for a 1" NPT for example)

 

I draw a 1.308" circle at the desired location and select "Enity" when I chain my

geometry.. That way the circle drives the tool and I don't have to worry about entering

the correct value in the operation.

 

I define my thread hob as an endmill.

 

It's diameter will be the small end of the thread hobb per manufacture's specs.

I don't waste time modeling visually accurate thread hobbs.

This is about generating gcode, not perfectly rendered eyecandy in Verify.

 

Depth is .1 to .3 deeper than specs per our customer's request.

 

We put 1.7833° in the taper field.

 

This typically produces a slightly undersized thread and the operator

uses CDC to bring it into spec.

[Rick46]

Ok I took pictures of master cam settings and also the nc code I use to cut my threads. I will post them when I get home cause I honestly want to know...

 

On a side note I'll be the bigger man and apologize for all of the arguing and bickering back and forth with crazy millman. I just know what my eyes see and that the results I get are correct. If they are not then hopefully when I get the code I have posted I can get some explanation as to why they have been coming out right not using taper..again apologizes to all..

[crazy^millman]

Believe it or not I care.

[gcode]

If they are not then hopefully when I get the code I have posted I can get some explanation as to why they have been coming out right not using taper..again apologizes to all..

 

our customer tests our 1" NPT threads to very high pressures and were rejecting our parts for failing pressure tests

when we left the taper setting out.

 

 

 

if you machine a really big NPT thread you can actually look into, you will observe marks on the Z+ side of the threads

where the tool nicks them if you leave the taper settings out.

 

Leaving the taper setting out has zero effect on how the thread gages.. it will gage perfectly

with our without the taper setting

 

but it has a huge effect on whether the thread will hold pressure or not.

[GoetzInd]

[Rick46]

of here are some pictures of the code that MC generates for me and MC settings showing no taper and this is how I cut my threads with great results. If I add taper it screws them up..so now maybe I can get an explanation on why what Im doing is working..oh and I use a .536 diameter for by cutter to follow when using this code to cut 1/4-18 npt threads.

 

hope the pics work cause its only way I can get stuff out of the minimum security prison I work in..lol..

[Manuel0822]

Really??!!! ROFFLMFAO after all this time this is the "darkest best kept secret of all times"????? LMAO.

 

I'm sorry if I look like an idiot but I was already feeling a little aggravated and fed up from people who just won't listen when everybody is doing their best to politely point them on the right direction.

 

To me it felt like I was watching somebody trying to get Wernher von Braun disqualified on his reasoning but then again this ain't rocket science, ain't it? Just 'nother dead gomn machining question.... 'MERICA Hell yeah!!!

 

You know what the funniest part is? Even thought there were code snipets shown as part of the answers, it sure looks like the person arguing never bother to even check them or he can't even tell the difference between them and his posted code.

 

What was the end result of that poll/thread about CNC Programmers needing some actual background other than a diploma?

 

Anybody remember the Simpsons episode when Lisa get's transferred to a different school and she no longer is the smartest and get's all depressed? I can still remember the dialog at the end when they are trying to decide whether to go back or stay:

 

Teacher: "So tell me Lisa, do you want to stay here and be a little fish on the ocean or go back and be a Big fish on bowl"

 

Lisa: "Big fish, big fish!!!"

 

Wasn't it Isaac Newton who said "If I have seen further than others, it's by standing upon the shoulders of giants". I know technology is changing every second but sometimes we just have to go back to the basics.

 

So after my rant is over, can somebody please point the answer for him??? It only took me 2 seconds to finally understand his method.

[Rick46]

if you have the answer with all your rants please share..by all means...

[gcode]

I see what he's doing.. but I'd never do it that way

 

the cycle time for that toolpath has got to be 10X what it needs to be

 

a 1/4-18 NPT thread shouldn't take more than 20 to 30 seconds at the most

[gcode]

this is how I would do it

 

This is one finish pass using the generic 3X post

 

%

O0000(T)

(DATE=DD-MM-YY - 22-11-13 TIME=HH:MM - 17:17)

(MCX FILE - T)

(MATERIAL - ALUMINUM INCH - 2024)

( T1 | MTB0375D0618-NPT | H1 | D1 | WEAR COMP | TOOL DIA. - .375 )

G20

G0 G17 G40 G49 G80 G90

T1 M6

G0 G90 G54 X0. Y0. S3378 M3

G43 H1 Z1.

Z.1

G1 Z-.41 F100.

G41 D1 Y-.0182 F22.17

G3 X.0682 Y0. Z-.3961 I.0317 J.0182

X-.069 Z-.3683 I-.0686 J0.

X.0699 Z-.3406 I.0694 J0.

X0. Y.0199 Z-.3267 I-.0378 J0.

G1 G40 Y0.

G0 Z.1

Z1.

M5

G91 G28 Z0.

M30

%

 

see attached X7 file

[Manuel0822]

I see what he's doing.. but I'd never do it that way

 

Neither would I that's why I would rather leave somebody else answer while I chill down a bit. The fall has finally made it to the south...

 

if you have the answer with all your rants please share..by all means...

 

You could compare the previously given examples or even the one Gcode is kindly giving you right now.

 

It only took me ***Hint 2 ***Hint seconds to finally understand his method.

 

IOW, check your pics

[Rick46]

while the feeds and speeds are not the ones I use just ones that were thrown in there when the tool was created for library purposes because I have to change them a lot from cutting alum, tool steels, and hardened steel..I normaly run this tool in steel at 30 ipm at around 4000 rpm and takes around 15 or 20 secs per hole. but if all of you are referring cause im starting from the top down instead of from the bottom up that's just a personal preference. I know climb cutting is the preferred method when doing any kind of machining but I choose not to in blind holes so Im not slamming into a hole filled with chips. I cant clean them out when im sitting at home drinking a cold one and my machine is running unattended. plus you cant climb cut in all situations. are you gonna climb cut engaging all teeth on your cutter when you using a 6 inch extension on your tooling..I bet that's will chatter like crazy plus shatter the insert.. @ manuel don't see what you have anything to be mad about you just chimed in on the situation with a bunch of rants and agreeing with other peoples methods if you got answer spit it out or leave your 2 cents at home. Im looking for educated answers here and waiting on one person that I believe to be very knowledgeable to chime in on this subject so if all you want to do is try and start argument which im to the point where if I cant get someone to give me an educated answer with out being a smart arse about it im gonna send a message to the moderator to see about closing this thread down cause all its turned into is a big mess...

[gcode]

Rick,

you're programming it like a single point cutter, spiraling down making a dozen passes to get to depth

These tools are meant to be used like an endmill cutting a wall, not a lathe tool turning a thread.

Talk to any factory rep in the business and they will tell you that..

Frankly, I'm surprised your method works at all, but it obviously does.

IMO, you are leaving a ton of money on the table, but if you're happy and your inspection department is happy, carry on.

There are dozens of very knowledgeable people watching this thread, and several have attempted to answer your questions,

If you can't get your answer here, perhaps you should contact Carmex tech support and ask them.

Sadly, I suspect you'll get the same answer there that you're getting here.

[GoetzInd]

Ok. Again. The reason you are getting what you think are good threads while not putting taper in the program is because the error on the size pipe threads you are milling is so small it is not easily seen. You comp the thread mill open until the gage goes to the proper depth and you think everything is good. Your customers will probably never see the error because it's either non-fluid or low pressure application and they are using sealant. Now, if you are doing very large pipe threads (as Gcode is doing), you will easily visibly see the error. Or, if you are doing high pressure dry seal applications, it will probably leak. This is what everyone has been telling you this entire thread and confirmed by the email I sent to carmex, your tool supplier.

 

Mike

 

edit: G, I was thinking that but he still isn't getting taper even if defined a tool as single flute.

 

[Rick46]

I'm at work but will respond back to this as soon as I get home cause I actually cut threads faster than the carmex guru that came with there sales rep..Jim I think was his name..he was amazed we were cutting well beyond there speeds and feeds as well as I'm only taking two radial passes and no axial depth cuts..but good info but still need my one question answered lol..thanks G code and mike..

[Rick46]

ok carmex sales rep and tech guru came into our shop Tuesday and went over the thread milling techniques with us because our shop is very new to thread milling as am I. we set up a work piece to cut 1-1/4 -7 threads using their feeds and speeds as follows. 5.52 IPM and 2538 rpm using one radial pass and 4 axial depth passes. there recommendations took 1 minute and 28 seconds to run and the threads had taper in them and had to run the path two more times to get the taper out. previously were running 50 IPM using the cutter as a single tooth thread mill and using one helical rough pass one helical finish pass and one helical spring pass and were cutting the threads in just under a minute like 53 seconds. going 2 inches deep. there were speechless that we were able to run their tooling that hard and end up with better threads than they had recommended using their speeds and feeds.. needless to say the purchasing agent was not happy that there tooling was not holding up to the standards there sales rep guaranteed. so a change in tooling may be in the future for our shop. as for the 1/4-18 npt threads are you saying if I feed from the bottom up using the taper in MC that the threads will come out properly versus coming down from the top of the hole not using taper.

 

on a side note the radial passes of any deep pitch cutter your gonna have to use a multi pass setup because if not that's a heavy cut to take and the insert wont hold up. the catalog im looking at recommends a minimum of two passes and up to four depending on the thread pitch on your larger cutters. we thread mill hundreds of holes at a time on plates and we want the inserts to hold up and have quality threads if this means using multiple radial passes going to depth using a helix or axial step down and its running un attended then that's money in our companys pocket not on the table..

[crazy^millman]

Im looking for educated answers here and waiting on one person that I believe to be very knowledgeable to chime in on this subject

 

You know I tried that and you would not listen. I have to say you really think very highly of yourself sorry us stupid people were not able to do so. They can close this thread, but this fact right here amazes me.

 

went over the thread milling techniques with us because our shop is very new to thread milling as am I.

 

And those of us that have been doing it for real and made it work correctly are not educated enough? Gcode's shop is one of my customers. Tk's shop is also one of my customers.

 

Rick I wish you the best and don't worry this less than educated person will not bother you again.

[Rick46]

@ millman I do think highly of myself always have and always will..anyone that thinks less than themselves has low self esteem in my opinion and needs a lift me up of some sort weather it be kind words or just someone to talk to. I always tell myself and even friends when there down in the dumps never think less of themselves because they are better than that and will pull through what ever it is that has them down. so yes Im guilty of reassuring myself as well as others with positivity in life. now if you've kept up with this thread I formally apologized for all the arguing that has went on between me and u mainly but others too. but now if we can forgive and forget as I am a forgiving man I don't know if you are or not for I don't know you. but I do know you are a smart individual and I have a solution to all this because like I said before I am new to this but am the only person in the shop that grasps the concept for I do most of the thread milling. so there for they come to me for answers on it. but Im having a problems grasping the concept of the not threads and the taper issue I understand what you are saying and maybe I didn't explain myself correctly when I explained how I was achieving my results without the taper. but any ways on to the solution. post a file with a simple diameter of .536 for a 1/4-18 npt thread using the the mill I posted pics of up above in previous posts so I can see whats going on and grasp the concept of milling the npt threads for they have more to them than regular screw threads do. if its off by .0017 the way im doing it and still works without taper I want to use the taper and have it be within .0002 cutting it the way its supposed to be. so if you want to really help then post an example file I can download in X6 format for the company I work for refuses to install X7 until its got the bugs worked out but that another issue of its own.. but X6 example file using this cutter mtb 0375 d06 18 npt mt7 milling it the way you are trying to expain to me and im not understanding so I can see what im doing wrong. and I will gladly tell you that you are right I was wrong. Im just the type of person when I see or hear something with my own eyes and ears I have to see it to believe it to see theres another way possible. and if you want you can pm me and I will gladly give you my email so you can email me the example file I ask for if you want to help me understand what it is im doing wrong. something is obviously close because its working now but I want it to be right and if you can show me that I will be greatly appreciative. I come to these forums out of all the rest available out there cause I know this place is full of knowledge but I just need to see whats being explained... thanks in advance..

[crazy^millman]

Rick I think we all can misundertand each other on these forums. I beielve it or not have been in your very shoes most of my life and I am the person with a smile on my face always trying to uplift people and better this profession as whole. I will be glad to put a sample file together. My email is always in my signautre and accept my aplogy for being to rash. I made my comments and should have just left them up there. I hate to have to aruge with anyone and I am man enough to admit when I am wrong, but I get paid very good money to be right. If I am right and my customer is wrong they do not pay me to agree they pay me to know my stuff. I have always told bosses, but mostly owenrs you do not want me to be right about you doing it wrong. I want you to feel comfortable with what I an many other people consider the correct way to cut NPT threads. Not becuase I am trying to be right, but becuase I know in my very soul it is the right way to machine them. I wish I could just keep my mouth shut and let you go on your merry ay, but just not in me to not try to corect anything I see is wrong. Men by nature are stubbon and we hate asking for directions and we hate being wrong. Shoot me an email and I will be glad to give you a sample file and help you figure out what in your application it is not going as you would expect.

[Guest]

Nobody will even know if an NPT thread is correct until it is exposed to max rated PSI. In which case either the test stand will be badly damaged/destroyed or worse, someone is injured or killed. All this corner cutting I'm seeing sends shivers up my spine.

 

We can all thump our chests and run down our list of accomplisments and pride and joy's but at the end of the day, some of us hold people's lives in our hands and they rely on us to make it right, to make it to perfection (or at the very least within spec). If we don't take that job seriously then we don't belong here doing what we do and we should just push a broom somewhere.

 

Over and out.

[mike93]

you need taper

[mike93]

do. if its off by .0017 the way im doing it and still works without taper I want to use the taper and have it be within .0002 cutting it the way its supposed to be. so if you want to really help then post an example file I can download in X6 format for the company I work for refuses to install X7 until its got the bugs worked out but that another issue of its own.. but X6 example file using this cutter mtb 0375 d06 18 npt mt7 milling it the way you are trying to expain to me

[mike93]

it is 2 clicks in parameters

[Rick46]

Rick I think we all can misundertand each other on these forums. I beielve it or not have been in your very shoes most of my life and I am the person with a smile on my face always trying to uplift people and better this profession as whole. I will be glad to put a sample file together. My email is always in my signautre and accept my aplogy for being to rash. I made my comments and should have just left them up there. I hate to have to aruge with anyone and I am man enough to admit when I am wrong, but I get paid very good money to be right. If I am right and my customer is wrong they do not pay me to agree they pay me to know my stuff. I have always told bosses, but mostly owenrs you do not want me to be right about you doing it wrong. I want you to feel comfortable with what I an many other people consider the correct way to cut NPT threads. Not becuase I am trying to be right, but becuase I know in my very soul it is the right way to machine them. I wish I could just keep my mouth shut and let you go on your merry ay, but just not in me to not try to corect anything I see is wrong. Men by nature are stubbon and we hate asking for directions and we hate being wrong. Shoot me an email and I will be glad to give you a sample file and help you figure out what in your application it is not going as you would expect.

 

Yes these forums, text messages, e-mails,etc.. can sometimes make people come across completely opposite of what they intend, its hard to see the emotion of ones intentions in a typed response. and I agree with you totally on men being stubborn as I am one of those guys that starts putting things together and when it doesn't work right then I seek the instruction manual for help.. I think we have all been guilty of that a time or two in life. I have to work a half day tomorrow so I will put together a sample file of my approach I am using and send it to you via e-mail and would greatly appreciate your input on showing me the correct way of doing NPT threads. what I'm doing now works but I take my job very seriously and I don't like doing things that are good enough to get by with I want to know I'm doing them the correct way and they are above and beyond good enough to get by. thank you for being patient with me through all this and again I apologize for all the misunderstandings we have had, and I respect you for not keeping your mouth shut and letting me be with what I have been doing. that's what makes you that guy, you go above and beyond no matter the situation and help people when you can. so don't be mad at yourself for that. keep your head up and keep doing what you do, because you are part of what makes this forum a great place and I'm sure you are a great part in the peoples lives that you are surrounded by on a daily basis. I hope you had a great Thanksgiving and I will be sending you an e-mail tomorrow in the afternoon with what I've got going and see what you suggestions you have on what I should do differently with it.

[mike93]

We use carmex solid carbide threadmills with the taper on the cutter and don't have this worry with inputting the taper in the taper angle box..just curious what brand tooling are you using that has 13 teeth or are u counting every tooth on the cutter if so that sounds like a low amount..I find using 1 tooth to work better and to enter cut by start at top of hole and to enter and exit at center rather then leading in and out of hole with radius to prevent accidental gauges..I know it's climb cutting this way but less hastle and retracts in my opinion also some controls will error out with a arc lead in with wear turned on..I've been cutting threads for long time and all different sizes and pitches and find this method to be sure fire every time and great finish..doing it the way above I can see why people are intimidated by thread cutting and why everyone that runs across a job that requires thread cutting comes to me for advice..all about the right tooling and cutter dia.'s as well as the way you approach it and it's as easy as drilling the hole to be thread

 

 

 

 

what----------------------