Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • 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!

Join Eng-Tips
*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.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

ModulusCT (Mechanical) (OP)
21 Feb 12 12:26
So we've had a question about our notes for some time where I work... Simply put, we're not sure how to do it. I have an idea of how it should be, but I'm unsure... Maybe someone here can help me out.

A few examples:

If I've got a tapped hole (#2-56 UNC 2B) with a depth of .18, I would think that the hole note should look like the following:

2X #2-56 UNC 2B <depth symbol>.180

... but what does that mean in regards to the drilling operation done before tapping? Is the drill tip going to be held to the same .18 depth dimension the tap is? If not, what is the proper way to control the depth of the drill? I would assume the following:

2X DRILL <depth symbol>.200
#2-56 UNC 2B <depth symbol>.180

,.. and if I want the hole fully threaded? Is that even possible? What about the drill tip? Is that part of the depth stated on the drawing? Or does it always go beyond the stated depth value by some amount?

Lastly, we use a lot of helicoils on our parts. How would one go about making a hole note for a helicoil insert while simultaneously communicating the parameters below:

10X DRILL <depth>.22
#2-56 UNC 2B
1.5X DIA. HELICOIL (TANGLESS)

Is that correct? Will the drill used for the .22 depth hole be the proper diameter to allow the end of a threaded fastener to pass through? Or will it be a pilot hole drilled for a #2-56 thread? I would obviously want to communicate that the drill diameter is whatever is appropriate for the helicoil insert.

Thanks for the help!

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

ctopher (Mechanical)
21 Feb 12 12:41
Call out what's needed to make the part.
I usually only call out the thd type and depth, unless it's starting on a counterbore surface, then I will add a dim on a section view to show the depth from t he correct surface.
I leave the drill depth up to the machinist to use the proper depth, unless the room below the drill tip becomes an issue.
It's usually better to have a little more info than not enough, but not too much to cause a machining or inspection nightmare.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

ModulusCT (Mechanical) (OP)
21 Feb 12 13:34
OK, so let's say the amount of material left below the drill tip is in fact, important?

If anyone can answer some of the specific questions I mention in my original post I'd appreciate it. Especially the part about the helicoils.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

drawoh (Mechanical)
21 Feb 12 13:40
ModulusCT,

   When you specify the depth of a tapped hole, you are specifying how far a screw or a thread gauge must go down into the hole.  If you have an issue with the depth of the tap drill, show a section or hidden view.  The issue for me is that I may or may not be determined to have a blind hole.  If the tap drill depth matters to you, add it to your section view.

   Don't tell the machine shop how to tap holes.  If they do not know this better than you do, you are in trouble.

   I would not specifically require tangless inserts unless I have a desperate requirement to eliminate helicoil tangs from my assembly.  Otherwise, I would just specify helical thread inserts.  If the tapped holes are not blind, tang removable will be easier, cheaper and more reliable.  I understand some shops give you the tangs in a little plastic bag, so you know they were removed.

   When you part arrives from the shop, your inspector has no way of knowing what tap drill was used, or whether you used tangless or regular helical thread inserts.  You don't care.  Your thread gauges should work.  You should get the end/bottom conditions you specified.  The holes should be in the right place.  

   When your inspector looks down into your holes, he should not see loose tangs.  You do not care how they did not get there.

               JHG

ModulusCT (Mechanical) (OP)
21 Feb 12 14:22
"If the tap drill depth matters to you, add it to your section view."

Does DRILL <depth>.20 indicate the same thing as the section view would? Does the drill tip usually get included in this depth value? I need to know because many times our blind holes are terminated only 20 or 30 thou away from the cavity on the other side of the part. We make enclosures for electronics and so, isolating the different PCB's within the enclosure is important.

Sometimes we say:

2-56 UNC 2B <depth>.200
DO NOT BREAK THRU

... which is OK, but sometimes we prefer at least .030 thou of material left beyond the drill tip to ensure there is no deformation of the opposite surface. I'm not entirely sure how to get this point across. If I did a section view would I simply attach one of the extension lines to the drill tip vertex?

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

ctopher (Mechanical)
21 Feb 12 14:26
Add the dimensions to where you need the drill to stop, let the machine shop handle the rest.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

Helpful Member!  MadMango (Mechanical)
21 Feb 12 14:41
Drill depth does not include the angles of the drill tip, only the full diameter.  On the following chart, you'll it is only dimensions to the full diameter, not the point.

http://www.barnhillbolt.com/specs/DimensionsHeliCoilInsertNF.htm

"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?

powerhound (Mechanical)
21 Feb 12 14:44
Typically, the hole depth does not include the tip. If you specify a .250 diameter hole at .500 deep then the hole should be .250 for the entire length of .500. If the tip is included in this then this will not be the case. Adding the DO NOT BREAK THRU note is effective as well. The same goes for tapped holes. The depth should be for the minimum amount of threads. Never tell the shop what size drill bit to use. They already know.  

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

ewh (Aerospace)
21 Feb 12 14:57
"DRILL" should not be specified;

Usually, a parts list contains the insert information; "HELICOIL" is a brand name and "INSERT, HELICAL COIL" unties the hands of purchasing.

The depth can't logically include the tip, as the dimension is not met there.  Duh.

Technically, the glass is always  full.

Helpful Member!  KENAT (Mechanical)
21 Feb 12 15:13
As others hint, don't specify processes just the end item per section 1.4 of the standard you reference.

I'd suggest something like

2-56 UNC 2B <depth>.200 MIN FULL THREAD
DO NOT BREAK THRU

If you need to spec minimum remaining 'wall' thickness then yes add a section and directly dimension the .030 MIN from the drill tip vertex to the wall.

Technically, if you don't show the through hole or explicitly say 'THRU' then the hole should be assumed to be blind but this is one of the situations I'd rather add extra annotation to be explicit.

As for helicoils you could treat the part as an inseparable assembly/detail assembly and just show the helicoil called up in a parts list and then have a reference call out to the helical thread and attatch the position FCF to that.  Then in the notes have something like "INSTALL PRESS FIT STANDOFF'S, STUDS, NUTS & HELICALS IN ACCORDANCE WITH THE MANUFACTURER'S SPECIFICATIONS."

Some will argue this is cheating, pushing the part definition on the fabricator etc. and it probably won't work in strictly controlled regulatory environments like defense/aerospace but for general industry may be fine.

Take a look at section 1.8.9 figure 1-34 for your depth questions.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

fcsuper (Mechanical)
21 Feb 12 15:25
I would often use a note "DO NOT BREAK THRU" on threads where the drill depth was critical to avoid a counterbore or other feature.  I was an extremely rare condition where I would actually specify the drill depth.  

I never specified the drill size, since you don't even really know the size.  Depending on material, and forming method, the drill size can vary quite a bit.  The final product is what you should be calling out, and that is the thread itself, whose callout alrady includes all the specs necessary to make a functional thread.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

KENAT (Mechanical)
21 Feb 12 15:30
If you must specify the drill dia - for instance if you need to allow another component to pass through it or it's an air channel in pneumatics or similar then I try to put a very loose tolerance on it to allow for the possible variations in tap drill due to process variation.

I reiterate that this is the exception not the rule - generally tap drill is not specked to US drawing standards.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

fcsuper (Mechanical)
21 Feb 12 15:43
KENAT,

Specs on thread clearance ID are already very tight when compared to normal machining processes.  I dealt with pneumatics too, never had an issue.  The biggest problems I had with threads was the manufacturing floor insisting on using teflon tap on NPTs destined for haz areas.  ::slaps hand to head::  Finally had to let reg agency ding us to get the point across.  But this is a whole different topic. :)

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

drawoh (Mechanical)
21 Feb 12 17:11
ModulusCT,

   The ASME Y14.5 standard explicitly shows that your specified hole depth is for the full diameter.  The tapered depth of the drill is below that.  

   If I am determined to have a blind hole, I write BLIND on the hole specification.  On some drawings, I have shown blind holes, and I have added a note giving the shop permission to break through.  

   If the bottom of your hole is close to the opposite wall, or you are doing something weird and non-standard, you need a hidden or section view to make things clear.  

               JHG

CheckerHater (Mechanical)
22 Feb 12 8:39
I went thru my entire copy of Y14-5M and didn't find any example of threaded hole being dimensioned.
Could someone point me in the right direction?
 
Helpful Member!  ewh (Aerospace)
22 Feb 12 12:16
Try ASME Y14.6

Technically, the glass is always  full.

ModulusCT (Mechanical) (OP)
22 Feb 12 13:16
"The depth can't logically include the tip, as the dimension is not met there.  Duh."

@ewh: Sir, if you're going to be rude, I'd prefer no response at all. If I misinterpret your meaning, than please disregard this reply.

To everyone else, thanks for the replies! You've given me plenty to think about. I ask these questions, not only for my benefit, but because usually I've got to convince my supervisor to follow a particular method that he's not familiar with (he's not familiar with Y14.5)... All of your responses really help me convey the importance of, say, a section view dimensioning the remaining material between the drill tip and opposite surface.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

KENAT (Mechanical)
22 Feb 12 13:23
Ease up ModulusCT, that wasn't rude it was humor, not great humor but then it is ewh!winky smile

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

CheckerHater (Mechanical)
22 Feb 12 13:37
ModulusCT,

Ewh just told me that standard you are looking for is not Y14.5.
 
KENAT (Mechanical)
22 Feb 12 14:01
ewh is spot on about Y14.6

Section 3.3.11 addresses just the issue you bring up, though it is a bit light on examples.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

ewh (Aerospace)
22 Feb 12 14:01
I apologize if I offend... that was not my intent; sometimes we over-analyze the problem when it is really quite simple if seen from a different perspective, such as that of Homer Simpson.

... and KENAT is right; I've killed my share of threads with some misplaced bombs before.

Technically, the glass is always  full.

CheckerHater (Mechanical)
22 Feb 12 14:13
Are you guys saying I am to buy another standard?

What is it, ISO?
ewh (Aerospace)
22 Feb 12 14:15
ASME

Technically, the glass is always  full.

Helpful Member!  ewh (Aerospace)
22 Feb 12 14:16
(duh!)

Technically, the glass is always  full.

CheckerHater (Mechanical)
22 Feb 12 14:25
C'mon, I was told you only buy 1 ASME standard, as opposed to ISO, where you have to spend several thousand dollars!
ModulusCT (Mechanical) (OP)
22 Feb 12 14:27
No harm done... I took your comment to mean that I was asking a dumb question or that I should have known something very simple. Which might be the case actually, hah. Anyway, like I said, sometimes I ask, not because I don't know the best way to do it (although, many times, I don't), but because I've got to explain my methods to a higher-up and you guys nail down many of the angles I don't think about initially.

So anyway, it sounds like the syntax I'm using is correct, and "DO NOT BREAK THRU" is sufficient in most cases. When the remaining thickness is critical, a cross section with a dimension from drill tip vertex to opposite wall is a good idea (something like .XXX MIN).

I understand that it's not a good idea to specify manufacturing processes on the drawing, but that seems counter-intuitive to me when you consider the fact that we put c'sink and c'bore symbols on our drawings regularly, which in some sense, is as much an indication of process as the term DRILL is. I leave out the drill diameter intentionally as I know, DRILL is sufficient to get my point across... which is, that I want the machinist to drill no deeper than the specified amount.

Y14.6... Got it.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

KENAT (Mechanical)
22 Feb 12 14:40
Counterbore and countersink have come to describe both the tools and the features created by the tools (or perhaps vice versa).

For instance, it is possible to create a counterbore feature using a separate drill/mill process from the initial hole.

So on drawings the symbol is specifying the feature created not the tool often used to create that feature.

Checkerhater, you need less standards for ASME, anyone saying only 1 is exagerating thoughwinky smile  Having worked both systems you can get most of the ISO stds into maybe 4x 4" binders.  For ASME you can get them into 1 or (may have been a 5x binder I don't have it on my desk right now).   

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

CheckerHater (Mechanical)
22 Feb 12 15:04
Kenat,

In the Brave new world (tm) you can fit most of the stuff on one disk:

http://www.iso.org/iso/pressrelease.htm?refid=Ref1262

And it cost less than Genium manual.
ModulusCT (Mechanical) (OP)
22 Feb 12 15:54
Last question... On a hole note, is it permissible to say the following:

<c'bore><dia>.095±.005
<depth>.025±.005

I'm asking because initially I thought that omitting the c'bore symbol would communicate the same thing. But in reality, I'm thinking that he would have no idea that we want to have a flat bottom unless we show, in a cross-section, or with the c'sink symbol, that we want otherwise.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

ModulusCT (Mechanical) (OP)
22 Feb 12 16:01
Let me ask that another way... We want a threaded hole with a flat bottom. Is that a threaded c'bore? Or is there a way to designate a flat bottomed hole that I'm not aware of?

Thanks (duh).

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

KENAT (Mechanical)
22 Feb 12 16:12
So, you want to specify a threaded hole where the tap drill is flat bottomed not 'V', but you don't necessarily care what depth the untapped portion is?

Nothing springs to mind in 14.5M-1994 (or 14.6) that addresses the 'flat bottom' issue.

I'd suggest a note saying 'flat bottom', and probably at least one section illustrating/clarifying that the flat bottom applies to the tap drill hole not the threaded portion.

(Note there can be a cost penalty to flat bottom holes, and certainly if you want the tapped portion itself to be flat you'll face issues.)

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

MintJulep (Mechanical)
22 Feb 12 16:29

Quote:

The depth can't logically include the tip, as the dimension is not met there.  Duh.

Just thinking like the bad machine operator that I am, and noting that drawings are not supposed to dictate process.

To drill a hole to a depth:

Bring the bit to touch the surface.

Set your zero or plunge stop.

Make hole.

No math involved if the depth is dimensioned to the pointy bit.
ewh (Aerospace)
22 Feb 12 16:42
Yes, but the conical surface of the pointy tip doesn't meet dimensional requirements, does it?

As to flat bottom, I don't recall the specs addressing it.  I have always added a reference pilot diameter then the note "FLAT BOTTOM" after (not reference), to be followed by the rest of the thread callout.  The pilot diameter is a reference dimension (more to note which feature of the hole needs the flat bottom) so as not to unnecessarily limit the machinist, as noted earlier.

Technically, the glass is always  full.

KENAT (Mechanical)
22 Feb 12 16:45
If it wasn't for the explicit mention of Y14.5M-1994 you'd have a very good point MintJulep.  

However, as that reference is made, and that reference has a very clear explanation in 1.8.9 & figure 1-34 about it being the depth of the full diameter I'm afraid ewh's point stands.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

CheckerHater (Mechanical)
23 Feb 12 6:29
MintJulep,

Two points:

1. After machinist makes the hole without thinking (pardon, using the math), somebody will have to check the depth; and checking "pointy" hole requires special equipment.

2. To avoid your drill dancing erratically before going into the material, you want to hit the spot with center drill first.

I do not insist my way is the only way; just a thought.
 
ModulusCT (Mechanical) (OP)
23 Feb 12 13:19
"So, you want to specify a threaded hole where the tap drill is flat bottomed not 'V', but you don't necessarily care what depth the untapped portion is?"

Not exactly, Kenat. I want to specify a fully threaded hole with a flat bottom. I'm OK with there being 2 incomplete threads at the bottom and perhaps a small amount of unthreaded hole due to tooling limitations.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

KENAT (Mechanical)
23 Feb 12 13:29
You want a fully threaded hole but you don't really?

2 incomplete threads mean it isn't a fully threaded hole by definition.

So, you basically do want what I said except that you want the depth of tap drill overrun minimized?

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

fcsuper (Mechanical)
23 Feb 12 13:32
For $2000 worth of ASME standards, you'll have to spend nearly $6000 for the equiv ISO standards.  It's also much easier to find information in ASME standards since there are fewer books to thumb through.  What do you get for the extra $4000 in ISO?  Many more title/author/contributor/copyright notice pages, many more under utilized pages (often where half the page is left blank in the middle of a section because of poor placement of images).  However, the extra large images are nice.  Also, there are presumed standard methods from the style established within the images, but sometimes without any support of the wording of the document itself.  

For the life of me, I still cannot find where display of quanity is explicitly stated to be "4 x", which is often presumed to the standard because of examples given in the images.  However, they've chosen such a non-descript font, it doesn't appear to be the same in all examples throughout the standard.

That's not to ASME doesn't have it's own problems, maybe I'm just used to them. :)

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

ewh (Aerospace)
23 Feb 12 14:19
I think a bottoming (or plug) tap?.
 

Technically, the glass is always  full.

ModulusCT (Mechanical) (OP)
23 Feb 12 14:36
"So, you basically do want what I said except that you want the depth of tap drill overrun minimized?"

Not just minimized, but clearly defined. So what I did was a normal callout:

<dia>.095 +.005/-.000
<depth>.25 +.000/-.005

And I added a section view with a clear view of the hole in question so that the flat bottom is clearly visible. I then added a reference MAX wall thickness dimension from the bottom of the hole to the cavity on the opposite side of the wall just to make it clear that no feature, drill tip or otherwise, should extend beyond the .025 dimension.

I think I'm all set now... I found a copy of Y14.6 as well, although, it's from 1978 unfortunately. It'll have to suffice until I can get my greedy lunch hooks on the 2003 standard.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

KENAT (Mechanical)
23 Feb 12 16:05
I'd forget putting it in the call out as it may be confusing.

I'd just go with directly dimensioning the max tap hole depth in the section view and hence not need to specify its diameter.  I'd make the call out my min full thread dimension - or maybe even put that in the section.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

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!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close