Reading a print for tap depth

Based on this drill and tap callout, how deep do you guys think it should be drilled and how deep should it be tapped? I'm wondering if I was taught this incorrectly earlier in my career. It's a blind hole and the total part thickness is 0.450 in this area.

Thanks,
Griffin

2020-01-15_08-37-56 by Griffin,

According to that print you drill to .35 (plus drill tip) and tap it any depth you like, tap depth isn't specified. For that part I would probably grind the useless tip off normal plug tap, send it to 0.340 and call it done.

You havent got much room there on that part, but sometimes (depending on customer) I drill a little deeper in blind holes to give a little more thread as many engineers dont actually realize how much you loose between bottom of hole and last full thread. Be careful though, if customer has a strict QC department do it exactly as drawing says. I remember once getting a non conformance from a tap drill that was 0.010 too deep lol. Glad that customer stopped sending work.

Griffin said:

Based on this drill and tap callout, how deep do you guys think it should be drilled and how deep should it be tapped? I'm wondering if I was taught this incorrectly earlier in my career. It's a blind hole and the total part thickness is 0.450 in this area.

Thanks,
Griffin

2020-01-15_08-37-56 by Griffin,

Click to expand...

normally On a blind hole they want perfect threads to the value giving +. Ie 4-40 .150 deep means just that, .150 MIN FULL THREAD deep anything else over that is fine as long as it doesnt break into the .350 drill depth.

is this a helicoil tap? then you would go buy the helicoil chart specs on 1x dia 1.5x dia etc etc

yours saying M4 has me curious, do you have attachment sheet that gives you a m4 designation or any notes on the print?.

to get thread depth of your part you go 1/pitch x number of turns. screw the Gage in till it stops then count the number of turns till it comes out.
when using a Gage or bolt to check in a blind hole make sure you grind the Chamfer off the Gage or screw so you get the proper reading with out bottoming out in the blind hole.

I would say your thread depth needs to be 4mm as it calls M4 but I dont do enough metrics and I would have to ask to clarify unless its on the spec sheet or print.
The reason I say ask is because you have a 8.89mm drill depth. but yet a 4mm depth is less than half. of drill depth. I am not sure if the Tap to M4 is 4mm or a call out from spec sheet.

American we do them all day long everyday and those are no brainers.

Delw said:

normally On a blind hole they want perfect threads to the value giving +. Ie 4-40 .150 deep means just that, .150 MIN FULL THREAD deep anything else over that is fine as long as it doesnt break into the .350 drill depth.

is this a helicoil tap? then you would go buy the helicoil chart specs on 1x dia 1.5x dia etc etc

yours saying M4 has me curious, do you have attachment sheet that gives you a m4 designation or any notes on the print?.

to get thread depth of your part you go 1/pitch x number of turns. screw the Gage in till it stops then count the number of turns till it comes out.
when using a Gage or bolt to check in a blind hole make sure you grind the Chamfer off the Gage or screw so you get the proper reading with out bottoming out in the blind hole.

I would say your thread depth needs to be 4mm as it calls M4 but I dont do enough metrics and I would have to ask to clarify unless its on the spec sheet or print.
The reason I say ask is because you have a 8.89mm drill depth. but yet a 4mm depth is less than half. of drill depth. I am not sure if the Tap to M4 is 4mm or a call out from spec sheet.

American we do them all day long everyday and those are no brainers.

Click to expand...

.70 is the pitch of the M4 thread...


I'd go with what mmurray70 said and grind down a plug tap or use a bottoming tap, you could always use a flat bottom drill if you're worried about punching through. On larger bolts I'll typically interpolate them and leave myself .005" clearance on the tap depth over the hole floor depending on the part. I rarely run more than one of something, so the time lost to interpolation isn't worth more than the laziness of loading some drills in the machine and I've got a solid reference on how far the hole goes down.

Not sure if you can contact the customer for clarification, but if not I'd say it's on them for not calling out tap depth. If you're as close to the called out hole depth with the threads as you can reasonably get I can't imagine you having issues especially considering the error on the drawing.

KC3KNM said:

.70 is the pitch of the M4 thread...


I'd go with what mmurray70 said and grind down a plug tap or use a bottoming tap, you could always use a flat bottom drill if you're worried about punching through. On larger bolts I'll typically interpolate them and leave myself .005" clearance on the tap depth over the hole floor depending on the part. I rarely run more than one of something, so the time lost to interpolation isn't worth more than the laziness of loading some drills in the machine and I've got a solid reference on how far the hole goes down.

Not sure if you can contact the customer for clarification, but if not I'd say it's on them for not calling out tap depth. If you're as close to the called out hole depth with the threads as you can reasonably get I can't imagine you having issues especially considering the error on the drawing.

Click to expand...

Yes it says that where it says tap. that has nothing to do with depth. other than to use for calculation when counting turns with a gage or screw. The Depth in Question is "Tap to M4"
only a fool would use a ground plug tap in a short blind hole as there is no need for it. Buy a good tap thats a 1.5 modified bottoming, there not expensive and there easy to get. plus they give you a better thread.

I am betting he can contact the customer, or its on the print. you don't go running a bunch of parts to WHAT YOU THINK IS right because you think its an error in the drawing and "ON them". I mean seriously dude

Delw said:

Yes it says that where it says tap. that has nothing to do with depth. other than to use for calculation when counting turns with a gage or screw. The Depth in Question is "Tap to M4"
only a fool would use a ground plug tap in a short blind hole as there is no need for it. Buy a good tap thats a 1.5 modified bottoming, there not expensive and there easy to get. plus they give you a better thread.

I am betting he can contact the customer, or its on the print. you don't go running a bunch of parts to WHAT YOU THINK IS right because you think its an error in the drawing and "ON them". I mean seriously dude

Click to expand...

Having a bad day?

There's nothing wrong with grinding down a plug tap. When I've got some parts to turn quick and I don't have the proper tap it's no big deal to grab a plug tap and grind it flat to make that part. I don't see how it gives a better thread, could you expand on that? If I'm wrong here or have something to learn I'd love to not do more dumb shit. That said, if you don't fuck the tap when grinding it down, there's nothing that's going to cause issues. I use TSC and take it a little easier and haven't had a single issue with fucked up threads (plus I didn't have to wait on a tap)...


M4 is not a designation for depth (at least I've never seen anyone callout M4 over 4mm when designating length or depth), the drawing also doesn't say anything about 4mm thread depth. I'm fairly certain whoever created the drawing made a mistake and for whatever reason threw in M4 where they should've called out an actual depth. Or maybe I'm wrong, which definitely isn't unlikely.

Yes, which is why I said contact them. However that's not always possible on an off shift with tight deadlines. We farm out a lot of parts and mistakes happen when our engineers miss something on a drawing. If they can't contact us it falls on us and if they guessed wrong I'll have to rework the parts in house. If you get a drawing that's incorrectly drawn up and you make it to that, are you responsible or is the person who sent it over? I know there's a lot of stories on here of it going both ways. But, you're right, maybe calling it on them and tapping to full depth isn't the best move... but how long are you going to sit on a job and tie up time for someone else's mistake? It's not clear cut. Tapping to full depth (or as close as possible) is more than likely what they're looking for. I've also seen engineers kick out drawings without a depth called out assuming you'll tap to the called out drill depth, for whatever reason.

KC3KNM said:

Having a bad day?

There's nothing wrong with grinding down a plug tap. When I've got some parts to turn quick and I don't have the proper tap it's no big deal to grab a plug tap and grind it flat to make that part. I don't see how it gives a better thread, could you expand on that? If I'm wrong here or have something to learn I'd love to not do more dumb shit. That said, if you don't fuck the tap when grinding it down, there's nothing that's going to cause issues. I use TSC and take it a little easier and haven't had a single issue with fucked up threads (plus I didn't have to wait on a tap)...


M4 is not a designation for depth (at least I've never seen anyone callout M4 over 4mm when designating length or depth), the drawing also doesn't say anything about 4mm thread depth. I'm fairly certain whoever created the drawing made a mistake and for whatever reason threw in M4 where they should've called out an actual depth. Or maybe I'm wrong, which definitely isn't unlikely.

Yes, which is why I said contact them. However that's not always possible on an off shift with tight deadlines. We farm out a lot of parts and mistakes happen when our engineers miss something on a drawing. If they can't contact us it falls on us and if they guessed wrong I'll have to rework the parts in house. If you get a drawing that's incorrectly drawn up and you make it to that, are you responsible or is the person who sent it over? I know there's a lot of stories on here of it going both ways. But, you're right, maybe calling it on them and tapping to full depth isn't the best move... but how long are you going to sit on a job and tie up time for someone else's mistake? It's not clear cut. Tapping to full depth (or as close as possible) is more than likely what they're looking for. I've also seen engineers kick out drawings without a depth called out assuming you'll tap to the called out drill depth, for whatever reason.

Click to expand...

The attitude its "on them" really sucks and its a piss poor attitude to have. you just dont run it with out being 100% sure and wait for an answer. its one thing if your know your customer and knows what they want, or its your own parts. but not knowing and using a answer on the net can be hazardous, as the people taking the guess's have no skin in the game.

typically if theres a min. call out then its open as long as you make that MIN FULL thread.
if theres only a depth for the tap lets say .200 deep then its full thread .200 deep plus or minus your tolorance what ever it is.

Blind holes generally have a call out for a few reasons most blind holes are short and they want xxx amount of minimum thread, sometimes they require you got to bottom of the minor dia. flat and that doesnt mean a modified tap going to the bottom, they will usually give a optional sheet that shows a counter bore a hair over the major size in which you have to use a key cutter to do it( we do a ton of these) then tap it. Then there some that want it "close" to the bottom well what exactly Close different meanings to different folks. close could be a standard bottoming tap, a modified 1.5 bottoming tap or even a hand ground less than 1.5 modified bottoming tap.
This one appears to have alot of thread for a blind hole. other reasons I have seen is they want to screw down something to a certain depth like a stop or bumper. or there putting a helicoil in it and dont want the guy putting in the helicoil to go to deep.

I dont do alot of metrics anymore, never seen a call out like that. unless they stated M4 meaning thread dia? then made a Rev change later clarifying it in RED thats its a M4x.7 theres a whole bunch of senerios the way it could be called out, with out knowing the customer, or seeing the whole print we will never know.

I had one customer about years ago, that they refused to call the customer if I had a Print question.I dont understand why maybe laziness or felt they were looking like a fool for asking, embarrassment.... I have never figured that out. they had the Same attitude as you have (its on them if its wrong). one day I got tired of the shit and reworking parts yeah they were paying me for it. so I called their customer direct of coarse telling My customer I wasnt going to run the parts unless I got confirmation and I want to talk to them.
of coarse my customer was wrong in his assumption of what it read. about a month later he and his customer and 4 of there engineers showed up at my shop going over all there print discrepancy that I told them about. it helped my customer alot cause they got so much machine work they actually had to fire there machines up to do my overload. not to mention they had no Discrepant parts
There engineers were from a major US medical company the engineers were foreign all but one was fresh out of school, they didnt understand simple things, not to mention they used solid works and snapped everything and rounded off 2 place decimal

Its never a bad thing to call your Customer to verify, scrap parts no matter whos fault sucks and doesn't give a good impression. Not to mention it shows your observant and competent.

BTW a mediocre and low budget plug taps ground on a m4x.7 going deep like that in a blind hole generally doesnt give a nice thread, chips are bad on most plug taps depending on the material, alum sucks with m4x.7 plug taps going more than .200 the m5 isnt much better the m6x1 6 isnt a problem

Not to git cought up in the drama...

I'd use a SF /mod bottom tap as was mentioned above and tap to just shy of the bottom and call it a day.


---------------

Think Snow Eh!
Ox

What is going on ?

Looks like switching up between English and metric midstream ?

Common.


-------------------

Think Snow Eh!
Ox

the answer to your question is, "Call the customer and ask them"

Even though it's a shitty ameture print, if you do it wrong it's on you.

I never call out a tap drill size- call out the thread (properly)_and a minimum depth for the thread. If its a thin part or on a thin wall or feature that you don't want to break thru and the needed thread depth is close to the feature thickness, then add a note "do not break through".

I see prints where the thread depth is called out to 3 places- that's BS- you will never get a part thru inspection with callouts like that. Keep it simple and functional. Like everything else on a good print- no guessing needed.

I get prints like this all the time from a few different customers. I've always just drilled so that the shoulder hits the specified depth, then tap it with a modified bottoming tap.

One customer got annoyed because I called to ask about something like this. If they don't specify thread depth, it's probably because it's not very critical.

I'd just ring up the customer or shoot them an email and move on to the next part while waiting for a response.

Been doing machining for 40+ years with 15 or so as a Manufacturing Engineer doing designing and drafting.
I try to get this through to young engineers and quality people. Just call out the thread with class and a minimum thread depth. If the drill can't break through then say that. All the extra stuff is just something for some uninformed quality person to reject. They do it all the time at my company. Inspector rejects thread because it's too deep
As far as grinding off plug taps. Only if you don't have the correct tap. I argue you this with a coworker all the time. He grinds off $80.00 Emuge specials just because he thinks he is being cute. The plug spiral point is ground that way for a reason. If it worked better flat, the tap companies would grind them that way.Drives me crazy

MachEng said:

He grinds off $80.00 Emuge specials just because he thinks he is being cute. The plug spiral point is ground that way for a reason. If it worked better flat, the tap companies would grind them that way.Drives me crazy

Click to expand...

No, not really. The point at the tip is a center, used to hold the tap when they grind it. Serves no purpose after the tap is made

It does seem to possibly help to give support to stringys as they wind their way up together on spiral point taps.

They take the time to grind them off of plug taps, but not SP.
Yes - the point is there for a male center to begin with.


------------------

Think Snow Eh!
Ox

Larry Dickman said:

No, not really. The point at the tip is a center, used to hold the tap when they grind it. Serves no purpose after the tap is made

Click to expand...

Exactly! I wasnt suggesting grinding a plug tap all the way into bottoming tap, just grind away the tip that doesnt cut anything, and maybe one extra thread if you like. This lets you get much closer to the bottom.

I tend to avoid bottoming taps unless drawing lists a full thread depth that requires a bottoming tap, or there is a note specifically saying to use bottoming tap.

You guys are brave, I never go closer than 0.050" to the bottom of a drilled hole with a tap! Even then I hit cycle start and walk away so I don't have to hear the crunching sound if something was a bit off.

I would call the customer to get a thread class and depth call-out. In past companies, we set up a drafting template that called out tap drill diameter and depth as reference then listed the thread, thread class, and depth as driving specs.

I think you are getting good advice on technical approaches to make the most of the tap drill depth but this looks like an under defined drawing call out to me.