Blind hole manufacturing

[BBprecise]

How do you guys manufacture blind holes with tight diameter tolerances?

 

We drill and line bore slightly deeper than print to make room for the chamfer on the reamer and chips. One of our customers just rejected some parts because of the small multiple depths in the bottom of the hole. They quoted us Y14.5M about the depth, but it doesn't control manufacturing of a feature and says nothing about going slightly deeper. The part is for Honeywell and we've done hundreds of Honeywell parts for our other customers and we've never had a complaint about how we manufacture blind holes.

 

Just looking for opinions and what not.

[crazy^millman]

The customer controls the process. Referencing a quality standard for manufacturing is just stupid. They want a perfect feature to the bottom then you go about the process to make that happen. If that means having to grind it in then you grind it in. You charge what the customer is driving the price to be. Once they see a 10% to 25% increase in the price of the parts you then tell them to revisit their quality requirements for the part. Blind flat bottom holes are not easy, but they can be done just requires some steps and methods to make it happen. 

[Guest]

Typically here if it's flat bottomed.....if it's flat, they want it flat

 

I helix bore it, size & depth depending of course

[Matthew Hajicek - Singularity]

If it's too deep for an endmill you can do a flat bottom drill after the normal drill.  If that won't hold tolerance and finish, then yeah, quote it for jig bore.

[robk]

ALWAYS follow customer specs. Never make your own decisions.

[BBprecise]

The holes aren't flat bottomed. The print shows drill point which is what the customer says is required. I have no problem meeting the customer requirements, just wished it made more sense. Like it was mentioned ASME Y14.5M spec is about how to dimension prints correctly and print interpretation and really doesn't pertain to manufacturing of a part. The method our process engineer and owner came up with still violates the drill point profile but they're going to submit it to the customer as a preventative action. There's a lot more that goes to this but you don't need to know that.

 

I was just inquiring how you guys deal with tight tolerance holes when the print only shows a drill point. I don't see how the ASME spec controls how to manufacture the hole. I was hoping someone would know of a spec or something that would prove my point. If it was specified as flat bottomed I know I can't drill deeper. but if it only shows a drill point and there's nothing preventing me from going a little deeper I don't see why we can't. Granted the other programmer that did these parts went .1 deeper with the drill and .05 deeper with the linebore than the dimensioned called out on the print (which is way deeper than I would have gone), and even the customers engineer says it wont affect the parts function, but their quality dept. is raising a stink. Live and learn I guess.

 

Have a good Thanksgiving guys. I'm on vaca. next week and plan to spend it all in the woods hunting with my son.

[jlw™]

Well, some one needs to not be a moron making dwgs with precision holes using their CAD's hole feature app.  They need to understand the processes required to manufacture what they design.  Just saying.  I've had to deal with this exact thing before.  EXACT THING.  I have ordered reamers ground with matching drill point and run it till it just kisses the floor.  You have to be very careful and I usually had them touch it off on a gage block on the part.  Keep in mind that it's going to cost more for special tooling and additional setup time.  Albeit not much, it will be reflected heavily in the cost of the part.  I briefly looked in my rolodex and didn't find the company who would grind the reamers for me like that but if I find it or it hits me I'll come back and post it.

[specv]

If its that critical we have:

Drill and ream with a modified reamer where the angle matches the drill angle and blend them together (coolant through reamer to push chips back)

Drill and bore with a  where the angle matches the drill angle and blend them together (coolant through bore to push chips back)

Use a dreamer so there is no subsequent operations needed.

 

We have also requested that they change the print to allow for a pilot drill size and depth.

[BBprecise]

I agree jl. Unfortunately we didn't get the end users (Honeywell) print, we got our customers print which was redrawn from Honeywells print (no idea why as we already know who their customer is). Our process engineer has actually contacted Fullerton (where we get most of our reamers) about having them grind drill point angles on reamers and they advised against it. Something about the 45º lead helps center and control size of the hole. They said they will grind a 118º if we request it, but advised against it. With the hole being blind and if I had extra room for chips I would normally use a straight flute reamer, but with no/very little room for chips I need spiral flute but they don't seem to be as available in as many different sizes as straight fluters without custom ordering them.

 

I would appreciate the info. Thanks.

[BBprecise]

Spec, we pushed back a little with our customer on this and they won't budge and keep referring to the ASME spec. It's mostly their quality dept. pushing back.

[Guest]

 

If it was specified as flat bottomed I know I can't drill deeper. but if it only shows a drill point and there's nothing preventing me from going a little deeper I don't see why we can't. 

 

I am going to focus on just this point here..

 

Many moons ago, a place that I used to work, we made the pins that mounted the blades to a turbine........we were held to a very exacting depth, even though the print showed a drill point....why, the full dia depth..... +.002/-.000   Weight balance

 

Sometimes, there are engineering reasons for something

[BBprecise]

I completely agree John. What I haven't mentioned is that our customer is shipping the parts back to us (for another altogether different reason) with a new p.o. and print to rework the parts to a change Honeywell has requested. Our customer is also going to change the hole detail on the print to match what we made so their QC will accept the parts. Which their engineer and sales dept. agree that what we did will not affect the part.

[crazy^millman]

I completely agree John. What I haven't mentioned is that our customer is shipping the parts back to us (for another altogether different reason) with a new p.o. and print to rework the parts to a change Honeywell has requested. Our customer is also going to change the hole detail on the print to match what we made so their QC will accept the parts. Which their engineer and sales dept. agree that what we did will not affect the part.

 

That is the best solution right there.

[specv]

Depending on the reamer (solid carbide or hss) we have even had a radius ground on them as well, if location is an issue we will semi-finish bore for location and ream for size. In your case boring might be your only option.

 

We do a lot of cutter grinding in house as well, i realize not many shops that have a tool/cutter grinder anymore.

 

We use: 

California Reamer

Hannibal carbide

Dihart

Mapal

[dstryr]

What is the tolerance on the hole and location?

[AMCNitro]

How deep is the hole?  And which diameter?

[BBprecise]

Sorry guys, was on vac. all last week. Location tolerance is TP of .003, size is Ø.1293/.130. Depth is .15 +/-.01.

[Guest]

.122 drill x .145 deep, helix bore with a 3/32 endmill x .150 deep....

[Newbeeee™]

The print shows drill point which is what the customer says is required.

The method our process engineer and owner came up with still violates the drill point profile

 

I was just inquiring how you guys deal with tight tolerance holes when the print only shows a drill point.

If it was specified as flat bottomed I know I can't drill deeper. but if it only shows a drill point and there's nothing preventing me from going a little deeper I don't see why we can't.

Not to be a jackass here, but this is your original paragraph but with a few sentences removed, leaving what I see as the important ones here.

Customer wants point - Boss deviated with no authorisation (bad boss...)

Drawing shows point - that would be what the drafty wanted - any deviation in writing please - If in doubt, ask.

Your statement showing drill point, and the fact that there's nothing preventing you going deeper, if the print doesn't say it, you can't.

 

Don't get me wrong, a lot of the time from a functionality point of view it doesn't matter, it's just the cad jockey hasn't specified it.

I'm fighting one customer at the moment with thread depths - specified as 5.00mm deep (doesn't say min - so that's +/-0.1mm tolerance then... )

 

 

But back to your original question - if it's flat bottom, drill and then spiral mill to take the bottom out, and possibly boring head if too tight to mill.

Jig grind would be last resort because another machine.

 

edit:-

I've told this story before I'm sure.

To me the most important note on any drawing is If In Doubt - Ask.

All of our customers have this note, but a few years ago, one customer removed it.

I queried why with the purchasing manager and he immediately queried it with the engineering manager.

5 mins later I gets a call back, and the reason was because the chief drafty was totally fed up with people querying their drawings...

[BBprecise]

Newb, my biggest issue is the customer is quoting Y14.5 which is a drafting/ how to interpret print spec. Doesn't control manufacturing process at all, which we cannot seem to get our customer to understand, but in the end they are the customer. The new method the boss and engineer came up with still violates the drill point profile (not as much as what we did originally) and we haven't verified with customer if it's ok or not, but the owner wants to make this the standard for this customer. We have done the same drill, linebore, and ream process on previous parts for them and they never mentioned anything (maybe it was because I did the programming and I didn't go as far beyond the print dimensions as the other programmer did on these parts) so it didn't draw the attention.

 

I wish our machines could hold +/-.0004 roundness so I could helix bore or just circle mill them, but they wont. The newest machine (an Akari Seiki which I hate, so they go and buy a used one this spring which is just as bad) is 4yrs old and it might be able to if I feed at 1ipm, but even then I doubt it. I can't get the powers at be to realize that better quality machines would save a lot of time because we wouldn't have to use so many boring heads.  From the factory they wouldn't mill a 1/4" wide slot +/-.002 on width without cutting it 3-4 times at 5ipm. We had a factory tech. (not distributor) and a Fanuc tech. here for 2 days to adjust the machine so it would circle mill a Ø3" ID fit round w/in .0015 at 30ipm. At the time our 2 Fadal vertical mills were 10yrs old and they would do that all day long. Enough ranting.

 

I was hoping somebody could give me something I could go back to customer with on how Y14.5 is applied and it doesn't control manufacturing, but that may not exist. All of our customers draw drill points for all of their holes, and those that need/want a drill point always specify it on the print.

 

Thanks guys.

[Guest]

The bottom line is Y14.5 does not in any way control "how" a part is manufactured.....it does control the features, tolerances and specifics of a parts.  There is no manufacturing component to it that I am aware of...

 

The place where I believe the customer was correct was, they drew a flat bottomed hole, they wanted a flat bottomed hole.....if they choose to accept something different, that would be a deviation, which should be rejected and noted......if they can change their print, that makes it all the better and the manufacturing becomes easier...

 

So, there is nothing you can go back to your customer with but there is nothing a customer could present that supports their point either...... 

[Newbeeee™]

Not having read the spec (we're all ISO over here), there's a link here

https://en.wikipedia.org/wiki/Geometric_dimensioning_and_tolerancing

 

But in reading this, they call attention to this section 'Dimensioning and tolerancing philosophy' which is worth a read.

 

My honest opinion is your Boss is on dodgy footings if he's still deviating from drawing without consent...

[Guest]

Not having read the spec (we're all ISO over here), there's a link here

https://en.wikipedia.org/wiki/Geometric_dimensioning_and_tolerancing

 

But in reading this, they call attention to this section 'Dimensioning and tolerancing philosophy' which is worth a read.

 

My honest opinion is your Boss is on dodgy footings if he's still deviating from drawing without consent...

 

I'm with you newbeeee, without prior approval, deviating from a print is a rejection.....regardless of whether it can be used or not

[BBprecise]

With how the customer is acting I agree the new process is still iffy at best, but he signs my paycheck so until otherwise told this is how he wants it done.

 

The print shows a drill point, but it does not specifically call out a drill point and it's not a flat bottomed hole. If it had been a flat bottomed hole we would have given them just that.

 

JP, that's the argument I made with our quality dept. (who originally got the NCR from the customer) and my boss, and they don't exactly see it that way and they wont push that back to the customer. I'll do what ever the boss wants in the end, but some times the customer is not always right. But if we're not going to stay perfectly within the drill point profile (although the new method is closer), it's no better than what we did originally in my book which irritates me almost as much as the boss doesn't see it that way.

 

We're ISO as well as AS9100 cert. and I'll admit it's been a long time since I've read the specs.

 

Not saying I disagree that the parts deviated from print, but there should be some flexibility when a feature profile is not specified or controlled by a note on the print in my opinion. Then again my opinion isn't always worth much.

[Newbeeee™]

 

Not saying I disagree that the parts deviated from print, but there should be some flexibility when a feature profile is not specified or controlled by a note on the print in my opinion. Then again my opinion isn't always worth much.

This is where the 'If in Doubt - Ask' comes in, IMO.