×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

How do I know what thread pitch I can use?

How do I know what thread pitch I can use?

How do I know what thread pitch I can use?

(OP)
In a nutshell,... im designing a cap that screws into a tube. I dont know the EXACT diameter of the cap where it will be threaded at the moment but but lets just say for example that its 2.34375".

How do I know what thread pitch I can use for this diameter? I've seen charts all over the place with nominal diameters, basic diameters, major diameters etc. But none of them come close to what I need. The closest I saw I think was 2.250 but the threads were to coarse think.

I am thinking I want something around 18tpi. But I dont know if I can do that?!?! I dont see why not? But how do I know what the specs are for this thread? I have to draft a 3D model of this part and I need to include the threads. I know the diameter of the part, the pitch, and angle(60deg right?). What about the rest of the specs like radius etc?

Can someone please explain this to me:( Thanks.  

RE: How do I know what thread pitch I can use?

You need to get your hands on a Machinery's Handbook.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of these Forums?

RE: How do I know what thread pitch I can use?

You can use any pitch you want.  It depends on your application.  For a non-standard, unified thread you can calculate the appropriate dimensions using the chart in the Machinery's Handbook.  To designate the thread on a drawing you give the major diameter followed by the tpi, the class, and "UNS" for "Unified Special" if it doesn't fall under a standard designation like UNC, UNEF, 12UN, etc.  

If you're nice, you then give the major, minor and pitch diameters that you have calculated.  The drawing callout might look something like this:

2 11/32-18-2A UNS
MAJOR DIA = ________
MINOR DIA = ________
PITCH DIA = ________

FYI, in addition to coarse, fine and extra-fine, there are several uniform pitch series.  One that might work in your application would be

2.25-20 UN

or even a secondary

2.375-20 UN

These are standard threads with dimensions in the tables.

Don
Kansas City

RE: How do I know what thread pitch I can use?

(OP)
Thanks guys! I went out just now and bought the 28th edition of the machinery handbook. I think I have enough info to figure this out. But if I have questions I will be back to ask;) Thanks again!

RE: How do I know what thread pitch I can use?

The FAQ I posted has a link to an online calculator that helps, though getting the formula and checking from first principles is a good idea.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: How do I know what thread pitch I can use?

(OP)
Ok. I did some reading in my machinery handbook and it is great but I am still not quite understanding it.

I want to know if the diameter of whatever it is your trying to thread effects the tpi at all? I mean im thinking 16tpi is 16tpi whether im trying to thread a .5" rod or a 3" rod. You know what I mean? The profile stays the same. Meaning the angle, the pitch, the flats(.125P & .250P). everything except the diameters. Is this right or no?

The machinery handbook said when choosing a thread that one should seriously try to use the standards in table 2 and if those cant be used then to use the threads in table 3.

Well,... I went looking in table 3 because i didnt see anything that I could use atleast I dont think. So I went to table 3. I saw there was a 2-3/8 - 16UN. I think I could use this for my application. So I did a quick search for thread milling cutters and found a site with some thread sizes. Of the sizes I saw 3/8 - 16. Check it out here:

http://www.harveytool.com/products/product_detail.php?product_id=70000&category_id=1&product_family=Thread+Milling+Cutters

Is that the size I would need? What is the thread size?!?! 16UN? If someone could just shine a bit of light on this that would be great. I never would of though that threading could be so complicated!

Just as a note,... what i'm trying to do is thread the ends of what I would like to be 2.5"OD x .125"wall acrylic tubes. I want to thread the ends in about .5". I want to make threaded caps that will screw into the threaded ends. The caps would be turn cut from scratch with a lathe etc to the spec's needed. The tubes will be cut down from larger extruded/ cast tubes. The tubes have a size tolerence of about .05" and the shape is a bit off too. So I would have to correct the shape of the tube for the tread milling process first.

Thanks guys.   

      

RE: How do I know what thread pitch I can use?

As I understand it, within reason/limits yes you can have almost any combination of dia & pitch as a UNS.  Obviously at extremes there become manufacturability issues.  I don't think I've seen a pitch over 100 TPI and that's mostly on relatively small (.25 or maybe #10) dia's.

The one you picked from the table as being a close fit to your dimensional needs is 2-3/8 - 16UN.  This is a 2-3/8 major dia with a pitch of 16 TPI.

The cutter you've selected is I think the right pitch but wrong diameter, 3/8" is a lot smaller than 2-3/8".

Although the thread form as such is the same for any given pitch, regardless of diameter, the actual thread is different for each combination of diameter & pitch.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: How do I know what thread pitch I can use?

(OP)
I understand what you mean about combinations being with reason. But what I dont understand is difference between the cutter thread size and the thread size of the part. I know that 3/8" is a lot smaller than 2-3/8. But what does the diameter of the part(2-3/8) have anything to do with the cutters thread size diameter(3/8)?

So from what your trying to explain is that I need to find a 2-3/8" - 16 size cutter?!?! How big is that! seriously. I dont understand that. I know with taps you have to have the exact size and in that case yes, that would be a big tap. But im talking about thread milling.   

    

RE: How do I know what thread pitch I can use?

It depends on your manufacturing process.  If your machinist is using a lathe, there is no worry about thread diameter and thread pitch.  They should be able to set-up the machine to cut any combination of threads.  If your machinist only has access to drill presses or mills, then you will need to find the proper tap and die set.

2-3/8" = the major diameter of the external threads, or minor diameter of the internal threads.
16 = the threads per inch, or TPI.

If you thought 20 threads per inch was coarse, then 16 will be even more so.  Also, I think you should only have to detail these threads in your model if you are sending the model to rapid prototyping for a molded component.  If this is going to be machined by a machinist, the call-out should be plenty to get what you are looking for is the machinist is worth paying.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of these Forums?

RE: How do I know what thread pitch I can use?

"2-3/8" = the major diameter of the external threads, or minor diameter of the internal threads."


2-3/8" would be the major diameter of external or internal threads.

Software For Metalworking
http://closetolerancesoftware.com
 

RE: How do I know what thread pitch I can use?

(OP)
The manufacturing process is thread milling via a cnc milling machine. I am not talking about taps and dies nor am I talking about cutting threads with a lathe using some kind of lathe bit. Thread milling. The thread milling cutters are smaller than the holes being tapped so that the holes can be thread milled. An example:

http://www.youtube.com/watch?v=NM5ZrgLOZVY

Now, if I had to tap the inside of a tube with 2-3/8" - 16 threads,... what cutter would I need? A 2-3/8" - 16 cutter? Thats a huge bit! Does the bit actually have a major diameter of 2-3/8"???    

RE: How do I know what thread pitch I can use?

A 2 3/8-16 tap has a major diameter of 2.375.

A thread mill to machine an internal 2 3/8-16 thread would have to be smaller than the minor diameter (2.307 min).  In practice, you'd be better off using a tool in the .750/1.250 range.  Your tool motion would be divided up into many more linear moves to machine the circle, which would give a better-looking thread.   You could run higher RPM's and machine the thread more quickly with the smaller tool, and probably with less tool pressure (important with tubing).
 

Software For Metalworking
http://closetolerancesoftware.com
 

RE: How do I know what thread pitch I can use?

(OP)
Soooo,.... are you saying that a 3/4 - 16 cutter would work?

RE: How do I know what thread pitch I can use?

If by 3/4-16 cutter you mean a 3/4 diameter thread mill with the appropriate grind or insert for 16 TPI, yes.

The length of the thread also has to be considered.  If you have to machine a thread 1.500 long, the tool has to be able to accomodate that.  Sometimes you have to go to a larger diameter tool to get one that has sufficient length while remaining rigid enough to produce a good quality thread.



 

Software For Metalworking
http://closetolerancesoftware.com
 

RE: How do I know what thread pitch I can use?

(OP)
Yes. The thread mill says thread size 3/4 - 16.

What do you mean by the length of the thread? How deep I have to go? I dont think I have to go any deeper then the standard .75 length. Im thinking more like .5" in length.

Another question. What's the difference between a 3/8-16 and the 3/4-16 cutter when it comes to making a cut like the one I need to make(2-3/8 - 16)? Why couldn't I use a 3/8 - 16 instead of a 3/4 - 16? The 3/4 - 16 has less deflection?

RE: How do I know what thread pitch I can use?

For a thread .50 deep in acrylic, the 3/8 cutter should be fine.
 

Software For Metalworking
http://closetolerancesoftware.com
 

RE: How do I know what thread pitch I can use?

(OP)
Thank you! Thats what I wanted to know. I will probably go with the 3/4-16 just in case I have a cut a full .75" deep. I just wanted to know if there was a difference form wise if I used a 3/8" instead. Thanks again.   

RE: How do I know what thread pitch I can use?

In acrylic, you could easily use that 3/8 solid-carbide Harvey tool to go .75 deep.

Good luck with your project.
 

Software For Metalworking
http://closetolerancesoftware.com
 

RE: How do I know what thread pitch I can use?

mrainey, thanks for the correction.  I shouldn't post after midnight, especially if I've been drinking. thumbsup2

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of these Forums?

RE: How do I know what thread pitch I can use?

(OP)
Yeah thats what I was kind of thinking. We'll see:) Oh,... was looking through the machinery handbook again and was studying the thread basic UN form and noticed that the crest and root flats are reversed for internal and external. I could use the same bit to cut external threads too right? I am thinking yes. I mean why not? But according to the handbook int and ext threads are different.  

RE: How do I know what thread pitch I can use?

I think I misunderstood the follow up question a bit too, sorry for any confusion.

As to the internal & external being different, I think it comes from the tolerances required to ensure a fit.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: How do I know what thread pitch I can use?


You only need to worry about the minutiae of the int/ext profile tolerance differences if you're making something to be interchangeable with some other manufacturer's parts or vice-versa that. You're making both parts to fit, so there's no need to worry.

I was recently stuck for a suitable thread mill on a large diameter thread milled job and used a lathe threading tool with a full form insert, I held the shank in a collet on the VMC and it did a great job. The only difference being that most thread mills are designed to do the full thread in one rotation overlaid with one pitch feed, whereas in my bodge, the insert only had three teeth so I had to go around several times with the appropriate feed to cut the required length.
 

RE: How do I know what thread pitch I can use?

(OP)
Thanks guys:) Thanks for the guide. I am going to look through it soon. Also im going to read through the thread milling section of the machinery handbook.

Does anyone know if you can use a cnc router with helix interpolation to thread mill really soft materials such as aluminum, copper, brass, and plastics? I'm thinking that single tip cutters would be perfect for a cnc router. What do you think?

Maybe the routers are a bit to fast. I'm thinking that would be the only problem?     

RE: How do I know what thread pitch I can use?


Regarding the use of a router for threadmilling, I have a lot of doubts!

Due to the geometry of the cutters, threadmilling tends to induce a lot of vibration, this is often exacerbated by the small diameter and extra length the job often requires. If you are forced to exceed the recommended cutter tip speed and you can't attain the required feed/rev and supply flood coolant, the tool life will suffer badly. Just take a good look at the figures in mrainey's very ggod link.

In general I would say that the spindle speed will be way too high and the whole thing will lack rigidity. However, depending on your router, you may be able to dry-cut your plastic 2-3/8 x 16 thread with a single point tool or a modified a muulti-tooth insert.

  

RE: How do I know what thread pitch I can use?

Hi all.
I am looking into advantages and disadvantages of different lathe tool posts. Could anyone please advise me on what i should be looking for. I have been tasked will improving the saftey and reducing the risks of our lathe tool posts at work. At the minute im trying to research different tool posts. Any help would be much appreciated.

RE: How do I know what thread pitch I can use?

Ryan, I think that should probably be a new thread.  I suggest you press the

Inappropriate post?
If so, Red Flag it!

Below your post and re-post as a new thread.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources