What's new
What's new

Tap Drill Hole notes

GatzW

Plastic
Joined
Nov 29, 2023
Hi guys, just throw in a question regarding hole notes, wondering whether these notes and clear enough for manufacturing and whether the drill sizes are correct? Thanks very much.
1710990964860.png 1710990993336.png
Also wondering when putting notes for sheet metal bending, do we normally specify the maximum bend radius or minimum radius, or it really depends? The note below is for 1.2 mm AISI 304.
1710991106864.png
 
You shouldn't need to specify the drill size just the thread class.
Most tradesman will have pocket guides or wall charts with tapping sizes.
maximum bend radius or minimum radius
I would prefer minimum as the female punch defines the minimum. No need to subtract material thickness from max rad.
 
I've never seen "clear" on a drawing. I wouldn’t list the thread size as it's not really necessary and just adds confusion, just call out the hole size directly. Before I saw the drill sizes referenced, I thought you were dimensioning tapped holes.

.180 is on the low end for an 8-32 clearance hole. I would go 0.185 +/-0.005" or #13 drill. Same with the 10-32. I'd go with the #3 (0.213") drill. A bit of wiggle room is good when working with sheet metal.

I am curious about the bend radius question as well. Following to see what answers develop.
 
This looks like a ProE/Creo print. "10-32 UNF 2B CLEAR" is saying that it's a clearance hole for 10-32, not a tapped hole.

ProE also gives out the tap drill size, free of charge. It's usually pretty consistent with what's on the Starrett chart on your wall. I realize that technically you should only specify the thread size and class, but I personally find it handy having that info on the print.

HOWEVER, for the clearance hole sizes (like in the print above), Creo always comes in a little tight. Instead of the standard 1/32 over on a 1/2-inch bolt, for example, it'll tell you to use a 33/64". On a 1/4" bolt, i think it defaults to F (.257"), which is not nearly enough clearance around a fastener, IMHO.
 
ProE also gives out the tap drill size, free of charge. It's usually pretty consistent with what's on the Starrett chart on your wall. I realize that technically you should only specify the thread size and class, but I personally find it handy having that info on the print.

There is one problem tho: depending on the organization you work for, there is a different tolerance class for holes and tapped holes.
IOW if you specify .190-32 UNF on the print, then the applicable tolerances come from the thread data.
If OTOH you specify .159 Through - Tap .190-32 UNF .500 deep, then the tolerance on the hole may come from your organization's spec sheet, which in case of Sikorsky Aircraft would be +.002/-.001
 
If OTOH you specify .159 Through - Tap .190-32 UNF .500 deep, then the tolerance on the hole may come from your organization's spec sheet, which in case of Sikorsky Aircraft would be +.002/-.001
If you spec'd the hole diameter like that, then yes, you could run into drilled holes whose tolerances are way-too-tight. However, what ProE specifies is not the diameter of the hole (which is in parentheses), but to drill with a certain size - i.e., use a #5 drill, regardless of the resulting diameter.

All that to say, Creo hole notes are not my favorite (why on earth do I need thread pitch information on a clearance hole?!), but I do like the handy reminder for the correct tap drill size.
 
I don't agree with the clearance hole callout. I want to know what size hole you want. The fact that it's a clearance hole for a screw is of no relevance. Size, tolerance, job done. For threaded holes, the size and the class, nothing more. OK, one more thing- whether or not the use of a form tap is OK. Though I prefer them for anything ductile, the nature of the crest makes it possible for the careless assembler to cross thread screws more easily than otherwise. OTOH, no more picking debris out of blind holes.

Only recently have I started to do precision sheet metal parts and it's much more of a rabbit hole than I ever would have thought. If you're bending moderate size parts out of mild steel, all the rules and tables work fine. Once you get into stainless or very thin/thick parts, you need to do some math. Read all the things Steve Benson has written for Fabricator Magazine. Start here- https://www.thefabricator.com/thefabricator/article/bending/sheet-metal-bending-calculation-basics and then read the "you may also like" at the bottom of the page. At that point you'll be able to specify something meaningful.
 
You didn't mention if you are working for someone or are self employed. For starters, I recommend reading through ASME Y14.5-2018.

In general I would not call out any type of machining process. i.e.- drilling, reaming, milling, edm, etc- Besides being a no-no to drawing standards, it could make you appear that you do not know how to design and/or you're a garage/basement business. However, If nobody else is ever going to see your drawings, then who cares? In that case, and if you're your own boss, your print can also serve as an internal process document.

When I used to design sheet metal and formed plastic parts, I would occasionally specify min or max inside radius if it mattered. I found out with all the outside sheet metal suppliers I used that preferred if gave them ID's, OD's and select important dims, along with a model, it worked out better for everyone. This was my experience but your suppliers may have different requirements.
 
Specifying a machining process is a no-no, but the work I do is so fussy that sometimes I have to. Being a sneaky you-know-what, I do it in a surface finish callout, where it's perfectly legal.
 
I don't agree with the clearance hole callout. I want to know what size hole you want. The fact that it's a clearance hole for a screw is of no relevance. Size, tolerance, job done. For threaded holes, the size and the class, nothing more. OK, one more thing- whether or not the use of a form tap is OK. Though I prefer them for anything ductile, the nature of the crest makes it possible for the careless assembler to cross thread screws more easily than otherwise. OTOH, no more picking debris out of blind holes.

Only recently have I started to do precision sheet metal parts and it's much more of a rabbit hole than I ever would have thought. If you're bending moderate size parts out of mild steel, all the rules and tables work fine. Once you get into stainless or very thin/thick parts, you need to do some math.
I am just now learning subtle differences in math for bending vs breaking metal. Breaking has the weird feedback once over bending. Bending is always 1/pi x thickness from inside as neutral axis for solid (rectangle cross section) metals. If you draw to that the flat always works out.
I can see how to make a hole called out if it matters, ie can be hand flame cut or must be drilled range. If it is clearance hole call out size only- the rest us up to fabricator.
 








 
Back
Top