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3D Model Tapped Hole Diameter

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Message 1 of 20
PeteMiller
6369 Views, 19 Replies

3D Model Tapped Hole Diameter

While trying to create a custom Heli-Coil Hole templet setting in Inventor 2011 for the Hole subroutine, I discovered an interesting quirk? If you examine Thread.xls the spread sheet that has all the thread data, you'll find that for a tapped hole Inventor uses the Minor Diameter value when it puts a hole into a part. Example, in sheet, "ANSI Unified Screw Threads", row 38, a 4-40UNC screw has a nominal body diameter of .112 and under the "U" column marked "Tap Drill" you'll find the standard ANSI drill diameter of 0.089, yet in a model, the value of the hole that is put into the part is the MINOR Diameter of .0849 (cell O38). This is uniform for any hole placed in a part, does anyone know WHY? If I send my model to my vender to use to profile the part for CNC, technically they would receive the wrong hole data. I was asked by my CAD Supplier would a 0.005 delta difference matter, and depending on the material that one is going to machine the part from it would. Aluminum isn't terribly finicky but if the material was 17-4 stainless or Kovar, it would matter. Since the table has the correct tap drill listed, why is that not used for the hole in the model? In the 2d drawing that is created, the ‘hole note’ can be modified to list the correct tap drill, why is the model different? When I get the Heli-Coil spread sheet worked out, I’d be happy to share it with anyone who’d like a copy.

19 REPLIES 19
Message 2 of 20
Anonymous
in reply to: PeteMiller

Open a model, go to document settings, under the modeling tab you can chose tap drill.

 

Message 3 of 20
PeteMiller
in reply to: Anonymous

John, Thank You (and to coin a phrase 'DUH!') although, when I change that setting (and why is that NOT in the hole feature itself...?) I get the following error message 'Drawing Manager thread representations are generated correctly only when Tapped Hole Diameter is set to "Minor". ' Any idea what that means?

Message 4 of 20
Anonymous
in reply to: PeteMiller

Don't have a clue.  You will have to try it and see. 

Message 5 of 20
pcunningham1
in reply to: PeteMiller

Basically what that means is that if you set the Tapped Hole Diameter to display as Major, then the hidden lines representing the threads will not be visible in idw drawing views, so they will look like unthreaded holes. Ridiculous in this day and age, but it is what it is.

Paul Cunningham
IV2008
Message 6 of 20
PeteMiller
in reply to: PeteMiller

I can understand if you had set the model to display the tapped holes as 'major', My question is 'why would you? As I stated in my original post, if I send a model to my vendor to fab, he's going to put drill hole in for the tap, not the major or minor diameter, so why not give them the right information to begin with? It is all about getting designs right the first time but I guess its a matter of preference, it just seems really odd.

Message 7 of 20
pcunningham1
in reply to: PeteMiller


@PeteMiller wrote:

I can understand if you had set the model to display the tapped holes as 'major', My question is 'why would you? As I stated in my original post, if I send a model to my vendor to fab, he's going to put drill hole in for the tap, not the major or minor diameter, so why not give them the right information to begin with? It is all about getting designs right the first time but I guess its a matter of preference, it just seems really odd.




Right off, I can think of two possible scenarios for using the larger diameter in the model:

1. To visually verify that the tapped holes aren't too close to another feature or edge, etc.

2. To eliminate perceived interference of threaded fasteners when doing assy interference analysis.

 

There is or was an effort to standardize imbedded mfg information , such as threads, finish , etc. into 3d models, but I don't know what became of it.

 

You'd think the Inventor team could come up with a way to:

A. Make all pertinent geometry of threaded holes visible in the model simultaneoulsly.

B. Always generate the threaded hole properly in the idw, regardless of what model display is chosen.

oh , and C. Make the warning messages understandable.

 

Paul Cunningham
IV2008
Message 8 of 20
PeteMiller
in reply to: PeteMiller

I agree Paul, those are valid reasons/concepts, I guess I've never had issues with holes being so close that I couldn't percieve of interference/fit problems before hand, perhaps just lucky I guess... 🙂

Message 9 of 20
pcunningham1
in reply to: PeteMiller


@PeteMiller wrote:

I agree Paul, those are valid reasons/concepts, I guess I've never had issues with holes being so close that I couldn't percieve of interference/fit problems before hand, perhaps just lucky I guess... 🙂



For the 'interference' bit, I was refereing to the Inventor Assy Inference analysis tool, which will interpret threaded fasteners as 'interfering' with their holes unless 'Major' diameter display is selected, IIRC.

Paul Cunningham
IV2008
Message 10 of 20
PeteMiller
in reply to: pcunningham1

Ah (chuckles) yeah, I had missed that one. actually when I do an interferance analysis, I prefer to know that the treads/hardware interfere, as I expect them to. If they don't then I feel I have other problems

Message 11 of 20
kstate92
in reply to: PeteMiller

To me, they should have two diameters on partially tapped holes: minor diameter per the selected thread standard with the threaded portion; pilot drill for the rest of the plain hole (assuming here: minor always > pilot). 

 

I would love to see a poll asking machinists / engineers if they have ever made or specified fully-tapped BLIND holes, because I wouldn't know why.  Maybe for threaded studs?

KState92
Inventor Professional 2020
AutoCAD Mechanical 2022.0.1
Windows 10 Pro 64 bit - 1903
Core i7-8700 32 GB Ram
Quadro P2000
Message 12 of 20
Anonymous
in reply to: kstate92

I don't even think there should be an option to fully thread a blind hole, in my experience it is close to (if not) impossible to produce with a tap,

 

If someone knows how to do this, let us in on it, please.

Message 13 of 20
kstate92
in reply to: Anonymous

There's Taper, Plug, and Bottoming, but I think that's more a set for hand tapping than production, automated setups.

KState92
Inventor Professional 2020
AutoCAD Mechanical 2022.0.1
Windows 10 Pro 64 bit - 1903
Core i7-8700 32 GB Ram
Quadro P2000
Message 14 of 20
PeteMiller
in reply to: kstate92

In the hole feature, if you click on the treaded hole function, there's a "full depth" check box, that option is to specific a partially threaded hole, such as "depth of hole .500" "depth of thread .375" I've done both mech eng as well as prototype machining, and there are times when you need a fully threaded hole such as when you have a very thin wall, and you (for whatever reason) can't break thru or have screw heads exposed, for say hermetically sealed parts. For reference a bottom tap will get you within a half a thread of the bottom of a hole, but usually its a clean up with a hand tap.

Message 15 of 20
shyfx
in reply to: Anonymous

Keep in mind that your drawings should not describe how to make the part, merely illustrate what the part's form should take.

To make a fully threaded hole can be done with operations other than tapping, EDM threading for instance. There is also thread milling, although I am not sure how far down to the bottom that can get.

https://www.youtube.com/watch?v=x3hEXA_q-dE
Message 16 of 20
PremTM
in reply to: shyfx

Hi,

 

I'm sorry for necroing the thread. I'm hoping someone could clarify a couple of things that are part of this topic.

 

First things first, I noticed that if you want to create a part with a threaded hole for a bolt or a screw you basically must use the Tapped Hole tool, otherwise if you first create a simple(clearance) hole and then thread it, you'll get some stupid outcome on the 2D assembly visualisation. Is there any use for such thing? I mean, under which circumstances would anyone thread a simple hole instead of creating a tapped hole?

 

Secondly, as it was previously mentioned here, the holes you make using Tapped Hole tool use the "Minor tapped hole diameter" and while trying to change it to Major you get a notification stating "Drawing Manager thread representations are generated correctly only when Tapped Hole Diameter is set to Minor". What exactly does it mean or what is the difference in outcome of these representations? Does switching from Minor to Major representation break the 2D sketch or something?

Sidenote: The option to change it is under: "Tools" tab -> Document settings -> Modeling

 

Thirdly, I guess every bolt or screw in its 3D model is used with "Major" diameter representation so it would be natural to set all the tapped holes to visualize the same, otherwise the 3D model looks broken and wrong when you view a halfsection of it. Would you suggest to do so or is it meant to look like you're pushing a big bolt thruough a small hole, at least in the 3D model?

 

 

Message 17 of 20
JDMather
in reply to: PremTM


@PremTM wrote:

... Would you suggest to do so or is it meant to look like you're pushing a big bolt thruough a small hole, at least in the 3D model? 

 


You should have started a new thread (pun intended) and included link to this thread.

 

Have you ever tapped a hole out on the shop floor?


Are you familiar with the difference between cosmetic threads and modeled threads as used in CAD programs?


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Message 18 of 20
PremTM
in reply to: JDMather

 

@Anonymous wrote:

You should have started a new thread (pun intended) and included link to this thread.

 


I see what you did there 😉

Yeah, I probably should have. Next time I'll remember.


@Anonymous wrote:

Have you ever tapped a hole out on the shop floor?


 

I'm not really sure what you mean by that.

 


@Anonymous wrote:


Are you familiar with the difference between cosmetic threads and modeled threads as used in CAD programs?


I suppose not deeply, but my guess would be that modeled threads are being used in items that are going to be parts of an assembly which requires some special attributes on them, but cosmetic threads are supposed just to show main features of a threaded part? No need to answer that, I'll dig into this topic soon.

Message 19 of 20
JDMather
in reply to: PremTM

 


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Message 20 of 20
JDMather
in reply to: JDMather

 


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