1/4 NPT thread mill

[within a thou]

The reasoon why you don't see the error is the sine of 1.79 degrees x pitch = .0017"

 

You should be putting the angle in like Ron suggested because on the larger threads you will get burned. Not sure why you would even want to use mcam to draw and define the tool then make a operation when most thread mill manufacturers offer software that will write the specific code for you based on which of their thread mills you are using.

[crazy^millman]

Not sure why you would even want to use mcam to draw and define the tool then make a operation when most thread mill manufacturers offer software that will write the specific code for you based on which of their thread mills you are using.

 

Because you do not have to copy and paste code into a program to run a part.

[within a thou]

Because you do not have to copy and paste code into a program to run a part.

 

And that is harder than all the work it takes to define tools, create geometry and so on? I get once it is created it is there forever but especially with tapered threadmills it is a lot of work to get the proper minor at the proper height where as the thread generator takes out all the guess work for you. To me seems a lot easier especially when you have multiple ones at differnt heights and levels to create points and run the generated code as a sub.

 

I am not trying to argue this point I am interested in why people do it with mastercam when the other tool is there already set up to go. To me a couple CTRL+C and CTRL+V is a lot easier than the alternative and it will be done right. Look through this entire thread their are more who are doing it wrong than right. Some can't even come to the agreement on whether the taper is needed or not.

[GoetzInd]

So every time you want to make a change to the program or there is a rev change you're going to copy that code back in and risk a mistake?

 

Mike

[within a thou]

So every time you want to make a change to the program or there is a rev change you're going to copy that code back in and risk a mistake?

 

Mike

 

Run it incremently as a sub.

[mikechvz]

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 cut

 

im using a Kennametal taper holder with the NPT inserts, Im just running it without adding the taper angle into mastercam, and its been working good and the thread-gage im using fits correctly. I had difficulty running multi passes, i kept alarming out on my machine when i was offsetting the wear, both running with the taper and without in the mastercam settings. Finally got things working, but it was a little challenging

[crazy^millman]

I have customers all over the world who demand complete Mastercam programs they can run. I do not have the luxury and telling them just copy and paste it from something else. It took me less than a minute to make that sample file in another thread how long does it take for you to define everything? You do the same work you create operation libraries with the point as the geometry. You then import the operation with everything defined and done in seconds. Put the work into the process and the process will work for you not against you.

 

Everyone is different that is the art part of programming. I tell people all the time it takes a certain amount of creativity to program a machine. Artist are called free spirits and I say machinist and programmers are in a sense the same thing. WE are free spirits that come up with all the different idea to make something, hold something and machine something. Machining is a much art as it is science. I say to a .0001 inspection of every part of the threads you are cutting incorrectly not using taper. Compare the output from the other programs that do put taper into their calculators and then tell me it is wrong to use taper? Sorry I would rather know I am doing it right than guess I am doing it right. Again go back to a single point tool and cut those thread, because the tool has taper does not mean it is 100% correct. It might be 90% correct and the gauge works, but I 100% am sure cutting taper threads with taper will make the best part possible. You are 100% sure cutting without taper does the same thing and unless we had a full 100% inspection report of the whole thread down to the micron level how will we know what is the correct process. I say Tomato and some say Tomato now reading that they read the same, but saying them depending on where you are from sounds different. Mathematically there is a difference so I will trust the math to support I am cutting correct part.

[Rick46]

why all your points are valid and correct. I know for a fact they make cutters with the 1.78 degrees taper on them and therefore not needed in the parameters in mastercam when using them. if you do so its compounding the angle and thus leaves stock in your threads.. if you were to cut the taper then try to use the tapered thread mill with the angle entered it wouldn't cut anything but air.. also carmex tech was in today showing us some new thread mill tooling and I presented him with the same question that's going on here about weather to use taper with there cutters or not and again if you have a cutter that has the taper form on it then you just run it straight down into the material and the taper will be formed from the cutter. I also tested this myself with and with out taper using a carmex tapered thread mill and you do not want to input the 1.78 degree if you want your threads to come out right. if you were using a single point cutter or a thread mill that does not have the taper on it then yes you do need the degree input in master cam, but if you use thread mills designed to shape the taper as well as the threads for you then its a no brainer and you will see real fast what happens if you do use taper on a tapered thread mill for NPT thread milling...

[GoetzInd]

How about this, model up some pipe threads. Make a custom tool that is an exact representation of a multi tooth thread mill WITH taper, verify it with and without taper entered and do an stl compare both times.

 

Mike

[djstedman]

No matter how you do it whether the angle is correct on the tool or not there will be error unless the toolpath is a spiral..

 

The error will likely be negligible and therefore unnoticeable for most applications but it will still be there..

 

Think about it .. the start point of the angle is at the bottom of the tool.. move the tool up one pitch without moving it out and the angle itself has moved up but will now not line up with the original angle since it hasn't moved out the amount the original angle has in one pitch..

 

I seriously find it hard to believe this is even being debated.. basic geometry..

[GoetzInd]

I seriously find it hard to believe this is even being debated.. basic geometry..

 

 

 

Haha kinda what I was thinkin....

 

Mike

[Rick46]

Works just like a traditional tap that can be used in place of thread mill..and they cut the taper just fine..and comparison has been done as you say and was shown to me no difference what so ever.common sense should tell you if you cut with a tool having draft or angle on it that if you add the angle in your path as well that your compounding it.. As far as spiral path goes all thread milling is done with a radial or spiral path with one pass or several passes just depends on your preference..and as far as I'm concerned I know what works and what the end result is on our materials using cutters with the angle on them and it's perfect and have seen demo comparing geo comparing what you guys don't want to seem to grasp all I can tell you is call carmex or your tool sales rep and have then explain the physics cause you will change your thoughts on the matter...technology has changed my friends and change is good...like I said before if I run the path with taper in master cam I get a screwed up thread..run it like manufacture recommends and threads are fine no error of any amount...

[GoetzInd]

Ok you win.

 

Mike

[Manuel0822]

Even though I'm with Mike to say I'm pretty sure you're stuck in your beliefs, here goes this sample straight from Allied's threadmilling software which you can use right from their website just for the record:

 

(THE START POINT FOR THE AMEC PROGRAM IS THE X, Y AND Z CENTER OF THE TOP OF THE HOLE.)

(YOUR PROGRAM SHOULD CHANGE TO THE THREAD MILL TOOL AND MOVE IT INTO POSITION.)

(INSERT THIS PROGRAM AT EACH LOCATION WHERE THE THREADMILL SEQUENCE IS DESIRED.)

(THE AMEC PROGRAM WILL SWITCH THE MACHINE TO INCREMENTAL, MACHINE ONE PITCH,)

 

(RETURN TO THE TOP/CENTER OF THE HOLE AND SWITCH THE MACHINE BACK TO ABSOLUTE.)

 

(PROGRAM NAME: AMEC_TMNK0500-NPT_11202013_18656)

(AMEC ACCUTHREAD 856 ITEM NUMBER: TMNK0500-NPT)

(PROGRAM CREATOR VERSION 4.0.0)

(THREAD TYPE: INTERNAL NPT)

(THREAD DIRECTION: RIGHT HANDED)

(PIPE THREAD SIZE: 1/2-14 NPT)

(MAJOR THREAD DIA.: 0.8320 INCH)

(LENGTH OF THREAD: 0.5340 INCH)

(TOOL DIAMETER: 0.4950)

(TOOL MAJOR CUTTING DIAMETER AT THREAD LENGTH: 0.4738)

(THREADS PER INCH: 14 NUMBER OF FLUTES: 4)

(MATERIAL: ALLOY STEEL 275-325 BHN)

(SPEED: 300 SFM FEED:0.0008 IN/TOOTH MAX RPM:10000)

(NO. OF PASSES: 3)

(PASS1: 50 PERCENT PASS2: 75 PERCENT PASS3:100 PERCENT )

 

(INCREMENTAL PROGRAM)

 

(3 PASS PROGRAM)

(PASS 1)

S2419 M03

M08

G91 G01 Z-0.5429 F50.00

G41 G01 X0.0753 Y0.0753 D1 F0.75

G03 X-0.0753 Y0.0753 Z0.0089 I-0.0753 J0.0000 F3.01

G03 X-0.1511 Y-0.1505 Z0.0179 I0.0000 J-0.1511

G03 X0.1511 Y-0.1517 Z0.0179 I0.1517 J0.0000

G03 X0.1522 Y0.1517 Z0.0179 I0.0000 J0.1522

G03 X-0.1522 Y0.1528 Z0.0179 I-0.1528 J0.0000

G03 X-0.0764 Y-0.0764 Z0.0089 I0.0000 J-0.0764 F6.02

G40 G01 X0.0764 Y-0.0764 F50.00

G01 Z-0.0892

(PASS 2)

G41 G01 X0.0824 Y0.0824 D1 F0.79

G03 X-0.0824 Y0.0824 Z0.0089 I-0.0824 J0.0000 F3.18

G03 X-0.1654 Y-0.1648 Z0.0179 I0.0000 J-0.1654

G03 X0.1654 Y-0.1659 Z0.0179 I0.1659 J0.0000

G03 X0.1665 Y0.1659 Z0.0179 I0.0000 J0.1665

G03 X-0.1665 Y0.1671 Z0.0179 I-0.1671 J0.0000

G03 X-0.0835 Y-0.0835 Z0.0089 I0.0000 J-0.0835 F6.35

G40 G01 X0.0835 Y-0.0835 F50.00

G01 Z-0.0892

(PASS 3)

G41 G01 X0.0896 Y0.0896 D1 F0.83

G03 X-0.0896 Y0.0896 Z0.0089 I-0.0896 J0.0000 F3.33

G03 X-0.1797 Y-0.1791 Z0.0179 I0.0000 J-0.1797

G03 X0.1797 Y-0.1802 Z0.0179 I0.1802 J0.0000

G03 X0.1808 Y0.1802 Z0.0179 I0.0000 J0.1808

G03 X-0.1808 Y0.1813 Z0.0179 I-0.1813 J0.0000

G03 X-0.0907 Y-0.0907 Z0.0089 I0.0000 J-0.0907 F6.67

G40 G01 X0.0907 Y-0.0907 F50.00

G00 Z0.4537

G90

 

So if I'm not misunderstanding the program, even the manufacturer shows a taper being programmed. If IRCC I believe my Carmex rep handed me a copy of an excel spreadsheet a couple years ago that was similar to what Allied has on their site.

 

I have always program using the taper and never had an issue, no matter what brand threadmill I can get a hold of, right now I have programs using Carmex, allied, stellram, emuge and advent and never had any issues so I guess there is nothing left to say than to each it's own.

 

If you you're doing it right the way you have it, then why bother?

 

Allied thread milling software

 

Anyways, HTH.

[htm01]

Ok you win.

 

Mike

ha,ha, that's what i have to tell my daughter when she does the same thing!

[Rick46]

I don't know if the "you win" comment was aimed towards me but thanks... ...But like I said earlier in the thread the best bet would be to take the advise of the "company technician, test technician or what ever title they are given" that you purchase your thread mills from for they can tell you the best and proper way to achieving your desired results with the tooling your using. They get paid big bucks to aid in designing and testing the tooling for their company, so they are going to be able to give you the best advice when using the tooling you purchase from them. I think this thread is full of useful and informative information but just some of it can be misleading and if used with wrong cutter can leave a person with undesired results. nothing more nothing less trying to be proven here..

[crazy^millman]

Edited by me.

Edited November 22, 2013 by Crazy^Millman

[Guyinthedesert]

So, later today I need to mill some 4-40's in Inconel. Should I use a neg taper to avoid having the holes get tight at the bottom?

[Rick46]

I don't know where you came up with the code and it was the companys research and design tech not sales rep that explained to me and also illustrated on his pc with a video of how it works, but I have to put food on my table as well and if I run opposite of what I am without the taper I'm gonna be standing in the unemployment line...and again for I don't know how many times I've said this you have to have the tapered cutter. We have code from carmex that I would have to take picture of due to not having internet but it includes no taper..I've even proven it by making test cuts with and without taper. So keep using your 25 yrs experience and do what works for you but I'm gonna run the cutters we have the way they are meant to be without the taper so I get correct results..I don't know how else to get this through to you I've got only few less yrs in the trade than yourself but I advance with the technology not stay set in my dinosaur ways...

[Rick46]

Tell me this then your 25 yrs experience how are my threads coming out accurately being cut with out taper and using code from carmex as well as mastercam code without taper. Tool defined as per specs in catolog and everything set correctly with the taper. Why does it come out wrong but yet if I use no taper wether it's code from carmex or mastercam it comes out right...answer me that correctly and I might take thought into what you are saying on this subject..people reading what they want and not the whole post and now your saying I'm getting code from sales rep..the whole reason we bought these cutters were because they cut the taper for you.but you explain to me how what I'm doing is coming out correctly and not just pasting some code up there for who knows what and then I'll admit I'm wrong. But when I've done it both ways and only one way works then what would you go with...no brainer there...

[crazy^millman]

Removed by me.

Edited November 22, 2013 by Crazy^Millman

[htm01]

all i can say is wow!

i have a brother that once told me "i don't care if i'm right or wrong i just love to argue"

[Rick46]

Got your nickel for u right here..remind me of a lot of people I've worked with in my 23 and lets say quarter yrs and they sure talk the talk but when it comes to producing they screw it up and end up in management cause they are bull sh@#%rs...and for one the code u posted is using the wrong cutter..but as to original question awnser it for them I didn't poet it..but if you want to get cocky about it then prove me wrong with your 5 cents as u put it..and if you can do so then great I'll learn two ways of cutting npt threads. I'm not arguing here but if everyone wants to call it that so be it..I'm just trying to get you to show me how it's done if I'm doing it wrong that's all if that angers you that I'm able to do it other than your ways then that's on you I care less who likes me in life..I just when it comes to machining complex parts my opinion is highly valued where I work and it's a big firm no hole in the wall shop .

[GoetzInd]

Rick, you brightened my day. Seriously.

 

Mike

[Guyinthedesert]

snip.

 

Can you just post a section of your code?