Proper Callout for Centerdrills 2

[vonsteimel]

Greetings,
I was wondering if anyone could enlighten me on calling out for center drills....

A lot of the old drawings here at my workplace just say "#3 center drill" but from what I remember, they actually had to be called out as below (couldn't find the depth symbol)....

2X Ø0.21 [5.5] x "depth symbol" 21/32 [17]
V Ø17/32 [13] X 60°
(#3 CENTER DRILL)

But I don't want to complicate an otherwise simple task. What do you use?
We're using the center drill locations to inspect total run out on some shafts. Otherwise they serve no purpose during use.

And obviously there is a tolerance that I have not pasted here...
Thanks,

VS

 

[JNieman]

IMO it's a redundancy issue. You're basically defining a #3 center drill dimensionally, and then also calling out a #3 center drill by name.

It would honestly be more practical to call out the #3 center drill and put the dimensions in parenthesis, as they are for reference more than the tool name is.

As you said, you don't really care much about the dimensions - just that you /have/ a 60d relieved hole for your centers to index upon. I would keep the annotation in the realm of the design intent.

_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms

NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[Tunalover]

JNieman says to call out the drill then reference the size. That's what one would expect to hear from a machine shop. What you care about is the function of the part which means to call out the hole size. I wouldn't reference the drill size at all. Reference data is worthless data because the parenthesis turns it into a non-binding requirement. What if someone can make the part cheaper using water jet? The center drill size number would then be completely meaningless to the fabricator.


Tunalover

 

[KENAT]

ASME Y14.5M-1994 section 1.8.12 & figure 1-38 applies if you work to that standard.

Posting guidelines faq731-376

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

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

 

[Tunalover]

Kenat-
Are you asking the OP author or me? I don't have the standard at hand.

Tunalover

 

[ctopher]

I don't see why callout a center drill on a drawing. It's a machining operation.
Do you leave a feature on the part by the center drill to be inspected?

Chris, CSWA
SolidWorks 14
ctopher's home
SolidWorks Legion

 

[ewh]

I've never actually dimensioned centerdrills, but have used them often by means of a note "CENTERDRILL PERMISSIBLE" (either a general note or one pointing to the feature).
Section 1.8.15 in the 2009 standard.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[KENAT]

It was a response to the OP Tunalover. If they work to that standard, and have a copy, then they could get the 'definitive' answer.

Posting guidelines faq731-376

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

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

 

[powerhound]

In your case, the preferred method by the shops I've worked at is just to indicate a center drill number and diameter where the 60 degree countersink intersects the end of the part. The center drill number isn't even necessary because the countersink diameter will dictate the size.

That being said, I have a sneaking suspicion that your drawing has a datum identifier attached directly to the shaft centerline. Is that true?

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Tunalover]

You can't go wrong by just calling out the countersink and through hole dimensions. The shop will know to look for a center drill of that size IF the part is machined.

Tunalover

 

[CheckerHater]

You don't have to show center drills on your drawing in general.
If you have no choice but to show center drills on your drawing, dimension them completely, as you shouldn't have undimensioned features on your drawing.
If you limit yourself to only specifying "drill number" it's a good idea to specify reference material a.k.a. "standard", so it's perfectly clear what exactly you mean by that

 

[ctopher]

CheckerHater, I agree.

Chris, CSWA
SolidWorks 14
ctopher's home
SolidWorks Legion

 

[JNieman]

The last example in Checkerhater's PDF is what I referred to. I believe that specifying tool dimensions is a way for conflicts to arise. While it is VERY unlikely that the standard for countersink combo drills will change, by keeping to a practice of calling out 'type' and the applicable standard, you leave your drawing safe for perpetuity as much as practical. While you may think of your part as being made for the next 6 months, some people may be working on parts that will be made for 40 years or more.

I do keep my 'industry' in my signature, for specific threads such as this, though. I do believe context/background of a persons profession affects their answer much. I know that when I switched from consulting engineering to a manufacturing environment that my beliefs/inclinations required adjustment. I'm glad to see the input from other 'types' on this topic, too.

_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms

NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[vonsteimel]

I was taught it must be completely called out as in my first post.

I could not find any depth specifications nor any tolerances concerning a "#3 Center Drill" therefore I don't see how it could be used a legitimate callout. The last page on the example specifies "ANSI/ASME B94.11M" which would work so long as everything is defined. However, I do not have ANSI/ASME B94.11M and If any of the subcontractors/machine shops do I doubt they have them readily accessible.

The drawing does have some GD&T, as I stated it is to check runout on a shaft. The problem is that its a common Ø1.25 TG&P shaft, which they can buy in lengths. Then they just cut it to length, hog a keyway and 2 centerdrills in it and DONE!. But since it was not turned using the centerdrills, they are often not along the center axis which makes them useless for checking runout with.

The last shipment we used a static balancer that has 2 sets of rollers. The shaft sat with a sets of rollers at each end and the runnout was inspected between them. It seemed to work well and would allow us to remove the centerdrill requirements.

I always put drill sizes in reference brackets to make the job simpler for the machinist, esp. if its done in house.

I always hesitate to use GD&T despite it being a superior way to dimension parts (i.e. a square tolerance zone created by standard dimensioning VS round tolerance zone using a position tolerance) because we deal with mostly local machine shop and are relatively low quantity (25 - 100 parts per year depending on the part). The owner also highly weights the price when creating an order. The cheapest always gets the order. period.
Most of the local machine shops rarely work with GD&T. Almost always, if a drawing goes out with GD&T I'll be getting a call from the shop asking questions, usually followed by an increase in price even if the allowance has increased through the use of GD&T (i.e. the position tolerances.etc)

There was a couple of guys who did a little study by sending out a series of RFQ's. Parts shown in only 3-views were sent, and also parts with 2 additional isometric views to show clarity were sent. The drawings with isometrics all produced cheaper quotes by a small but significant percent. (I cant remember much detail about this test/study) But I'd bet it would be the same with GD&T. Anyway, thats for another thread....

My conclusion is that I should keep the centerdrill callout as is.
Thanks,

VS

 

[JNieman]

I understand your apprehension to using a centerdrill feature as citing it by commercial nomenclature. I realize there is no fully defined and tolerance'd standard for the tool (that I know of) such as one would find for bushings, tooling balls, and other standard parts found at vendors like Carr-Lane.

There's a good reason for this. A center drill is not a precision cutting tool. It is not to be relied upon for precise geometry. It is a piloting tool, more than anything. It is never used as a finisher for precise geometry. If this is what you were going for then maybe it is inappropriate for you to use a center drill in the first place. Perhaps you missed the forest for the center-drilled-tree.

If you require on-center 30 degree tapered holes in the ends of the part on centerline, precisely, to a set dimension, and precisely located, then maybe it's best to pilot with a center-drill and touch it up with a small inserted boring bar for finishing.

This goes back to whomever stated it being better to simply call out the geometry rather than tool - and let the manufacturer connect those dots.

However, by drawing this part with complete center-drill geometry and calling it out with such precision - you take away the manufacturer's ability TO connect those dots. You force them to use a center drill but require more precision than a center-drill may allow. Perhaps the best design to convey the proper usage and intent would be to simply draw, dimension, and constrain the 30 degree taper alone, without the combo-drill geometry for the pilot, and provide a note to add "pilot drill permissible" or something similar.

That might make the part easy to make while getting you the reliable part you require.

My 2 cents.

_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms

NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[CheckerHater]

So guys buy pre-machined precision stock, then add center drills to it "to check run out" and then blame GD&T. Did I get it right?

Must be heavy case of Fridays, please ignore me

 

[vonsteimel]

JNieman, there is no tolerances posted for the callout in my first thread therefore precision cannot be determined. Your reaction to such a callout is the same reaction that many machinist have when they see a string of GD&T. That is to automatically assume there is a greater requirement for precision. That is not the case. The tolerances given on the drawing allow plenty of room to connect the dots. In-fact, dimensioning the geometry rather than calling out a ANSI/ASME B94.11M (as in the example) provides more room for dot-connecting, as tunalover specified in his post above.


The precision required for the hole to function is fairly low. All I need is a place a "Tail stock" will fit so that runnout can be checked. Center-drills are perfect for this. The precision is needed in locating the hole, to ensure it is close the center-axis to not throw off the runnout inspection. A job to which the center-drill is well suited. If there was a legit callout "Drill to fit standard Tail-Stock", I would have used it... But no such callout exist to my knowledge....


CheckerHater, I'm not sure where you got any of that, but I take it you don't get into PO/RFQ much aye? As JNieman mentioned above, a persons professional background can have quite an effect on their "beliefs/inclinations". It is not uncommon to find machinists who aren't familiar with GD&T. Even I have to pull out my ASME book every once and awhile since I don't use GD&T too often. This is an important thing to remember when you want to keep your parts cheap. It does have an effect on price.

Thus far, we have not had any parts fail the runnout inspection other than because the centerdrills were off. Even then there were only a few that flunked. We discussed the issue with the subcontractor but since the problem could be easily resolved in-house, we did not send them back. Once we put them on the static balancer, they all passed. This is why were considering removing the center-drills all together.... But I was still curious about the best way to call them out.
Thanks,

VS

 

[MikeHalloran]

Given that you're buying TG&P stock, it makes zero sense to pay someone to precisely locate and drill centers from which to check the stock. A runout check tells you only the precision to which the centerdrills were located.

If you're worried about camber in the stock, you can check that by rolling the cut and deburred shafts on a surface plate. No center needed; just a feeler gage.

If you insist on retaining a runout measurement, mount the shaft with a collet in a spindexer at either end, or just keep using the balancer blocks.







Mike Halloran
Pembroke Pines, FL, USA

 

[Tunalover]

vonsteimel,
If fabrication vendors charge more just because they see a feature control frame on a drawing (and ignore the size of the tolerance zone) then it's time to shop around for new vendors! GD&T is far from new (first version out in, what, 1966?) and any shop that doesn't understand it is FAR behind the times. Just saying...


Tunalover

 

[CheckerHater]

I did not pick at anyone's professional background. As others already explained to you, adding non-functional features just to apply GD&T to them is not an answer.

You don’t have to add separate feature just to create datum.
You can designate line or the area on the existing feature that will be used to create datum. This is called “datum target”. Look at Para. 4.24 in Y14.5-2009, especially Fig. 4-52.

This will be more in line with using static balancer, or a collet as Mike suggested.