Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

NPT Issues

16 REPLIES 16
Reply
Message 1 of 17
SeanFarr
6332 Views, 16 Replies

NPT Issues

Good Day All,

 

I am modelling a pin that is ported in one end for lubrication purposes using Inventor Pro 2012. A 1/4" pilot hole is drilled to a depth until the intersecting hole is reached. Then the same hole is drilled 1" to allow for a 1/8 NPT fitting for the autogreaser to attach to. I know the NPT threads only go down about 3/8".

 

After researching what size to drill for a 1/8 NPT fitting, I found that drill size R (.3390) is to be used. So using Inventor hole command, I tried to create this thread. But for some reason inventor uses .313 as the tap drill size?

 

I am creating another pin that will require a 1/4 NPT fitting and the tap drill size to be used is 7/16, but inventor again uses a different value .422 (27/64)?

 

I don't require the model to show the eact thread, and on my drawing I will just use the hole annotation to show what I want and the shop can determine what tap drill size to use from their references....But why are these number so different?

 

 

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
16 REPLIES 16
Message 2 of 17
JDMather
in reply to: SeanFarr

When I worked out on the shop floor - we always used this chart

http://www.brokenbolt.com/images/starrett-inch-metric-tap-drill.pdf

with minor variations for class-of-fit considerations.

These values seem to be close the Inventor values.

 

I found a reference to Whitworth pipe taps in Machinery's Handbook that was closer to your values.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 3 of 17
karthur1
in reply to: SeanFarr


@SeanFarr wrote:

... 

After researching what size to drill for a 1/8 NPT fitting, I found that drill size R (.3390) is to be used. So using Inventor hole command, I tried to create this thread. But for some reason inventor uses .313 as the tap drill size?

 

I am creating another pin that will require a 1/4 NPT fitting and the tap drill size to be used is 7/16, but inventor again uses a different value .422 (27/64)? 

 


This is something that AD has wrong about the NPT threads. I dont have a good answer for you on this. Its a catch 22.
If you use the values in the table, then the threads will model correctly, but the tap drill will call-out wrong in your thread notes. Thats just what you ran across.
You can change your table to get the correct tap drill callout, but then some of the NPT sizes will not be modeled correctly. This is the way that I have my table.
Its been like this ever since they included NPT threads, and will probably be this way forever. They need to use a different column for the tap drill information.
Message 4 of 17
SeanFarr
in reply to: SeanFarr

Ok Thanks JDMather and karthur,

 

It seems that there is nothing wrong with my model then,reading from your replies. Whichever value inventer decides to use for tap drill size, it is ultimately up to the machinist to decide what tap drill is best to produce the wanted NPT. As long as my detail drawing states what NPT is required.

 

Correct me if I am wrong but when annotating a thread, tap drill size is not required, just the thread info, ex. 1/8 - 27 NPT, unless of course there is a class of fit consideration as you mentioned JD.

 

Thanks Again


Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 5 of 17
mrattray
in reply to: SeanFarr

If there is a non-standard class of fit then you still shouldn't call out the tap drill. You would call out the fit. I have never once called out a tap drill size.

You don't tell the machinist what to do, you tell the machinist what product you need made.

Mike (not Matt) Rattray

Message 6 of 17
Anonymous
in reply to: SeanFarr

We don't specify tap drills on our drawings at all.

We mostly use roll taps, which require a larger tap drill than cutting taps.

So my advice would be to leave the tap drill off the drawing and let the machinist decide, as you said.

 

Message 7 of 17
SeanFarr
in reply to: SeanFarr

Thanks All!!

 

Still kinda new to the forum, can I accept more than one reply as solution or only one?? haha

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 8 of 17
kstate92
in reply to: karthur1

I suspect at Autodesk, 'NPT' stands for 'New Part-Timer', as in: give the thread stuff to the newbie, 'cause it's boring and not part of the next sales campaign bulletpoint list.

 

On a personal note, I wish NPTF were outlawed.  Making them consistently right seems to be more art than science, and pressure testing with them means you're wearing the peaks flat before they even ship.  I suspect the real reason they persist (like in-laws that won't leave) is that the fittings are cheap (like the in-laws) compared to the alternative systems.  I have seriously thought of advocating line-item charges, at least on our quotes.  Oh, you want NPTF ports? Here's the extra cost you'll have to pay, and yes it is just slightly more than the price difference between an NPTF one-piece screw machine part versus a real, modern hydraulic fitting!

 

Grease fittings I guess we're stuck with, but why isn't at least 1/4-28 straight thread the standard by now?

KState92
Inventor Professional 2020
AutoCAD Mechanical 2022.0.1
Windows 10 Pro 64 bit - 1903
Core i7-8700 32 GB Ram
Quadro P2000
Message 9 of 17
mrattray
in reply to: kstate92

Is it just me or have you gone on this anti-NPT rant at least once before?

Mike (not Matt) Rattray

Message 10 of 17
kstate92
in reply to: mrattray

Yeah... a lone voice, crying in the wilderness.  Or a crackpot to be avoided like a skunk that wants to cuddle.

KState92
Inventor Professional 2020
AutoCAD Mechanical 2022.0.1
Windows 10 Pro 64 bit - 1903
Core i7-8700 32 GB Ram
Quadro P2000
Message 11 of 17
msklein
in reply to: JDMather

I  just looked at my old "TAD" screw chart and realized that it matches what AutoDesk has, but not what Starrett say's. But then most of the companies I've worked for only listed the thread callout and left the tap hole Up to the shop. Just not specifying the manufacturing  processes but end result only, specifying thread class forces the shop to use the correct drills.  Guess i'll have to make sure in future i don't use those numbers off of the "TAD" chart or Software.

MSK

Message 12 of 17
hosford
in reply to: SeanFarr

The tap drill sizes look as though they were expecting you to use a npt taper reamer prior to tapping.

Thaddeus Hosford
NUC9i9QNX i9-9980HK, Win 10 Pro 64
Nvidia GTX 1650
Inventor 2021
Message 13 of 17
acad-caveman
in reply to: msklein

Being a machine shop rather than a design/engineering entity, I would like the opprotunity to perhaps quietly say something about this subject....

 

 

First, please, unless you have an absolute need to call out the diameter of ANY tapped hole - NPT or any tapped hole - do not include the diameter of the hole on your drawing.

This means that any UN, UNF, UNJ, UNJF, NPT etc threads should not include the "suggested" hole size.

Any and all machinist or shops worth their salt knows what the hole size should be, and separatly indicating them will lead to confusion or even a possible price difference.

 

Second, if your thread is a special thread (  UNS or the like ), please do not ONLY include the tap drill size, rather include

any and all parameters for that feature!!! That is all limits of minor, major, pitch diameters.

This will avoid phone calls and / or scrapped parts.

 

Third, for plated parts where your requiremens are critical, please indicate the maximum deviation for the pitch and minor/major diameters for the plating allowance.

Do not assume that the machinist will get it right, not because he/she doesn't know how, but because the lack of clear indication will often result in near fist fights with people in the inspection department.

 

Fourth. If possible, please try to model your threads with a BASIC dimension for minor dia. on an internal thread, or BASIC major dia. of an external thread.

Inventor has the ability to use " tap drill" in the modeling environment for tapped holes. I have edited my Threads.XLS file so instead of the default values are actually calculated by excel in this manner:

((major - minor)/2 + minor)

This way any thread will have the exact basic diameter modeled and the CAM software will know exactly what to do with it.

 

Fifth. This is kind of a peeve in this side of the pond ( US), but even tough standards do not require the pitch ( elevation ) callout of a metric thread, if it is not too much trouble, please, do include the complete thread specification of a metric thread. That is to say call out M10x1.5 instead of a simple M10. There are many reasons for this, but the most important would be confusion elimination. We all know the plain Mnn callout means standard ( coarsest ) thread, but that is still open for questions. Case in point, I have custom made taps for M10x1.75 and M10x2 threads.

Similarly, some (most) taps around here are marked as M10x1.5, so a newbie might ( actually always ) stands there  with a dumb look on his/her face wondering if that is in fact the correct one to use.

 

Now for NPT threads, whatever inventor does with them is useless, but so is Solidworks.

They are slightly more cumbersome to make right, but with a little knowhow the machinist can do them with ease, or a decent CAD jockey at the machineshop knows how to draw them right.

Call them out as "whatever"-NPT and let the shop modify the drawing to suit their needs. It will likely be modeled as a revolved feature to indicate the taper, and will be adequately longer ( deeper ) to acomodate the tool used to machine it.

 

I appreciate your audience, and now I get off my soapbox to go back being a simple blacksmith......

 

 

 

Message 14 of 17
Vlad.Makarov
in reply to: SeanFarr


@SeanFarr wrote:

After researching what size to drill for a 1/8 NPT fitting, I found that drill size R (.3390) is to be used. So using Inventor hole command, I tried to create this thread. But for some reason inventor uses .313 as the tap drill size?

 

I am creating another pin that will require a 1/4 NPT fitting and the tap drill size to be used is 7/16, but inventor again uses a different value .422 (27/64)?



Inventor contains alot of wrong information. The content library has incorrectly sized parts, NPT taps are off, O-rings are off and I could go on. To top it off, a great deal of this bad info has been there for years. I trust my certified machinists with 20-30 years experience before I trust this wet behind the ears program.

 

______________
Inventor Pro 2012
Vault Pro 2012
Message 15 of 17

You can change the number in the table.  But then the thread does not look correct.  You will need to change all the numbers to the correct sizes.  I was having the same problem with 1/8-27.  I needed .339 drill.

Message 16 of 17

This thread was created 10 years ago! Back when I was at a different company. I quit doing CAD work and went jackleg/stoper muckpile mining.

 

I forget what this was even for, But I assume the correct changes and updates have been made since 2012. I am back behind the screen now again also!

 

Cheers!

 

 

Sean Farr
Product Designer at Teksign Inc.
Inventor 2016 SP1
Dell Precision 3660
i7-12700 @ 2.40GHz-4.90GHz
32GB DDR5 4400MHz RAM
NIVDIA RTX A2000 6GB
Message 17 of 17

Mark,

Correct.  If you adjust the value in the Tap Drill column, the threads will not look right in the model.  Were you able to get both a correct looking thread AND the correct call-out on the idw? I was not ever able to do that and just gave up.  I now use the tap drill callout that is in the OEM spreadsheet.  The tap drill values in the OEM Thread.xls are for holes with an allowance for a tapered reamer. I do not know of anyone that uses a tapered reamer ahead of an NPT tap.... but that is how it is. BTW, this is from Inventor 2020, but I added the note circled in RED.

 

 

karthur1_0-1665574916871.png

 

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report