Proper Callout for Centerdrills
Proper Callout for Centerdrills
(OP)
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
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





RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
Tunalover
RE: Proper Callout for Centerdrills
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Proper Callout for Centerdrills
Are you asking the OP author or me? I don't have the standard at hand.
Tunalover
RE: Proper Callout for Centerdrills
Do you leave a feature on the part by the center drill to be inspected?
Chris, CSWA
SolidWorks 14
ctopher's home
SolidWorks Legion
RE: Proper Callout for Centerdrills
Section 1.8.15 in the 2009 standard.
“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV
RE: Proper Callout for Centerdrills
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
Tunalover
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
Chris, CSWA
SolidWorks 14
ctopher's home
SolidWorks Legion
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
Must be heavy case of Fridays, please ignore me
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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.
RE: Proper Callout for Centerdrills
Bill
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
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
RE: Proper Callout for Centerdrills
_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms
NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5
RE: Proper Callout for Centerdrills
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