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

 

[BillPSU]

Adding dimensions to a center drill is not necessary. Are you going to inspect the centerdrill for size and location? Are you going to reject the part over the centerdrill. I think not. Having a note, 'centerdrills are allowable' is all that is required. I've actually machined a shaft which was over 600 pounds and a no. 3 centerdrill was insufficient for the application. I have also seen shafts which were multiple tons in weight. The centers were very large.

Bill

 

[Tunalover]

BillPSU,
I disagree. The drawing should show the end-item including all the pertinent dimensions. Calling out a center drill imposes a specific process on the manufacture of that part. The drawing is supposed to stay free from processes and show only the end-item result. What if someone had a different way of creating the feature? Calling out a center drill tells them they can't do it the way they want to!


Tunalover

 

[ewh]

ASME Y14.5-2009
1.8.15 Where machining centers are to remain on the finished part, they are indicated by a note or dimensioned on the drawing. See ASME B94.11M.
(emphasis mine)

There is nothing wrong with specifying machining centers on the part without specifying dimensions, if called out in a note. Or course this infers that the geometry is not shown on the drawing, where they would require dimensioning.

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

 

[JNieman]

I think the crux of our back-and-forth originates in the fact that many of us are talking about nominal everyday conditions where the truth of the design is that a note of "centers permissible" accomplishes everything perfectly and elegantly, however the OP is in a situation where he desired to deliberately call out centers of a certain general size. That is obviously an exceptional circumstance to which many of us have digressed into the discussion of 'norms' in industry. I fell into that at first, before I understood what purpose the OP was attempting to serve. Now I think it's simply a fallible approach and a rather Sisyphean verification of geometry.


_________________________________________
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]

Mike, thanks for the advice. I believe I will indeed remove the centerdrills and use the static balancer from here out. We do not own a suitable surface plate. Just a bunch of steel work benches that I wouldn't trust. My formica desktop would be about the flatest thing we've got but I'd rather inspect them in the factory.

I think JNieman said it best. If we have to check runout using the centerdrills, then they perform an important function and therefore must be called out properly (in one of the two methods discussed above). This is what drafting is all about. Its not just about conveying information to the machinist/subcontractor.etc, but also about creating a clear, consise legal document between us and the subcontractor.

We didn't always have a static balancer and therefore had been using a tail-stock to check runnout. The centerdrills were not added to apply GD&T. It was added to allow us to inspect it. Doing such a thing (adding a feature to permit/aid inspection) is uncommon but not unheard of. To add a little background, these parts used to be machined on a lathe and needed centerdrills as a result. The guy before be had just dimensioned "#3 centerdrill". (yes, that callout worked but is not legal unless followed by "ANSI/ASME B94.11M" as discussed above). Simlilarly, it did not contain any GD&T but just specified in the notes "0.005 Total Runout"

If I don't plan to use the centerdrills, but just want to let the machinist know they can machine them required for a process on there end, "centerdrills are allowable" would be fine. On the revised drawing, I'll put in the notes "centerdrills are allowable but are not required". Otherwise they may assume we still want them.

There seems to be a disconnect between theory and actuality when it comes to drawings, dimensioning, GD&T, quoting & pricing. We generally shoot to order any given part just once a year. Whenever it gets time to order our metal/machined parts we send RFQ's to 4 - 5 shops. I'm not saying all machine shops are not familiar with GD&T, but many of the smaller ones (that aren't too big to take our small orders at a reasonable price) do not deal with it on a frequent basis. One of the biggest shocks to me after leaving school and entering the workforce is difference between theory and actuality.

Thanks,

VS