Hole Notes (ASME Y14.5M-1994) 4

[ModulusCT]

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]

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]

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]

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]

"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]

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

 

[MadMango]

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 to make the best use of these Forums?

 

[powerhound]

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]

"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.

 

[KENAT]

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

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[fcsuper]

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]

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

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[fcsuper]

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]

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]

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?

 

[ewh]

Try ASME Y14.6

Technically, the glass is always full.

 

[ModulusCT]

"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]

Ease up ModulusCT, that wasn't rude it was humor, not great humor but then it is ewh!;-)

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[CheckerHater]

ModulusCT,

Ewh just told me that standard you are looking for is not Y14.5.

 

[KENAT]

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

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​