Question about using the term 'THRU' on a drawing, when dealing with a pair of intersecting holes 1

[MASawtell]

Have an example of something that has me a bit confused. Have a threaded hole that will 'break through' the one side of another hole in a part, which will be shown as a 'blind hole' on a view in a part. Normally, I will put a depth that will not affect the other side of the other hole, but enough to pierce the hole completely. I have a colleague that insists that I would be putting 'THRU' for the depth, but have had the understanding that 'THRU' tells the machine shop to drill a hole completely through a part. Before anyone asks, I have a copy of ASME Y14.5-1994 (Re-affirm 2004) and ASME Y14.5-2009 in front of me, and have seen the Section 1.8.9 (1994) and Section 1.8.10 (2004) for Round Holes, which is clear on blind holes, but it would be nice if there was additional standards I could use in the upcoming debate.

 

[CheckerHater]

I wanted to suggest posting on this forum but looks like you are already here.
The first and foremost your call-out should be unambiguous, that is, do not have more than one interpretation. If your drawing actually contains section view like in your example, the situation is not so bad though.
For the reasons you mentioned “thru” is not the best choice and is not favored by ANSI/ASME standards.
If you look into your copy of Y14.5-1994 Fig. 5-11 you will see designation “both sides”. Will “one side” solve your problem?

 

[KENAT]

thread1103-217231
thread1103-156220

Posting guidelines faq731-376

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

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

 

[drawoh]

MASawtell,

Your section view tells the story. I would specify neither THRU or the depth.

SolidWorks distinguishes between THRU and THRU ALL. Your hole is THRU. I still would never trust the hole specification to guide the machinist. The section view is unambiguous.

--
JHG

 

[CheckerHater]

Here is another look at the problem:
When you specify something like “thru one wall” or “to the cross-hole” you assume that one hole is actually made before the other, so essentially you are suggesting a process, which technically is a big no-no.
From purely functional point of view, your hole has to accommodate the screw, meaning to have proper size and sufficient depth.
So if we take “functional” requirement seriously, we are to specify the depth of hole AS IF the cross-hole never existed.
Other ideas?

 

[randy64]

In this situation, we use THRU TO HOLE on the callout for the smaller hole.

CheckerHater, I would disagree that THRU TO HOLE suggests a process. It is simply defining the end product. If the machinist wanted to calculate the depth of the smaller hole and drill it first, he/she can do that, but in the end the smaller hole hole will be thru to the bigger hole.

 

[Belanger]

When you specify something like “thru one wall” or “to the cross-hole” you assume that one hole is actually made before the other.

A small nit-pick...I don't see this as the case. It is simply saying that the dimension (i.e., the hole itself) is to continue through space into something else. It's not a directive about mfg.

It's like saying that a profile tolerance extends between two points. That doesn't literally mean that the manufacturer must chronologically make that surface beginning at one point and concluding at another -- it might actually be a molded part that is made all in one shot.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[CheckerHater]

If the machinist wanted to calculate the depth of the smaller hole and drill it first, he/she can do that

The problem is that machinist absolutely positively must know how deep to go.
End every time machinist is forced to do any unnecessary calculations creates an opportunity for error.
So, talk to your local machinist and ask which dimensioning scheme he or she preferred, A or B?
JP, you are invited to speak to the machinist as well.

 

[MASawtell]

Couple of notes as I 'gird my loins' and get ready to debate this morning:

1) The sample that I used is not the style I am working with for the drawings (i.e. no hidden lines in views and very few section views)

2) Fellow designer in my office pointed out that machinists have to deal with the length of their tools, so calling out a particular depth can be 'tricky' because the machinist has to compute tool lengths

Regardless, appreciate the advice on this, trying to keep these drawings as compliant to Y14.5-1994 as I can.

 

[JNieman]

CH:

In our shop it is perfectly /intuitive/ to call out "THRU TO BORE/HOLE/POCKET" etc and is used commonly by a great many of customers and also for our own internal design and drafting practices. It's a second-nature callout in my experience in machining as well as the feedback from our machinists.

There is no expectation that machinists will not have to do calculations from time to time, even if they are programming at the machine or running a manually machined part. You can minimize it, but "design intent" goes a long way rather than giving depths. You don't give a crap if he drills a 1/4" hole to the center of the 2"d cylinder that's getting a 1" bore through it. You just want to make sure it breaks totally through the wall. So it betrays your design intent to specify otherwise, and may induce inefficient machining if he actually programs it to cut 1" deep in a 2"d cyl when he can get away with 3/8" depth.

_________________________________________
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]

JNieman,

I have nothing against intuitive practices of your shop, it's just they don't belong in the print.
Your process sheets, set-ups, programms, QC charts, whatever. It is reaally great if holes meeting together will be taken into consideration.
But is there really functional requirement for small hole to stop at the cross-hole? What if tomorow the cross-hole will change or move? What if we have different dash-numbers with different cross-holes?
The list can go on and on.

 

[powerhound]

As a machinist, I can tell you that neither I nor anyone I work with would ever make the assumption that one hole must be created before the other based on that verbage. What determines that is the part geometry. In the case of the OP drawing, the cross hole in the wall would certainly be drilled second regardless of what any note says.

I am constantly amazed at how simple minded some engineers consider machinists to be. I had an argument with an engineer who insisted on putting stacked limit dimensions on prints with the smaller value on top simply because they thought that since the machinist will read (if this particular machinist actually could read) from top to bottom and expect the lower value to be on top. If they put the larger value on top, the machinist might think it was the smaller value and run the part as such.

Please...a little credit.

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

 

[KENAT]

Pretty much all this territory was gone over in the links I posted above.

I disagree about it implying manufacturing process, and despite at one point being convinced to do so I hate putting a depth dimension on for the intersecting hole when there is no resultant depth to measure. Simply putting 'min' doesn't work because it can end up allowing the hole to continue on past the intersecting hole which may not be design intent. I suppose the real requirement is some 'min' dimension that breaks fully into the cross hole but then 'do not break thru far side of cross hole' or some such but that can start getting messy.

This is one of those simple things that if you look at it long enough can get quite complex/messy.

Posting guidelines faq731-376

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

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

 

[CheckerHater]

KENAT,
In case of threaded hole like in OP you can say "thread MIN, drill MAX" to make sure hole is not going to far.
This is one of the situations that better be dealt with on the case-to-case basis and using verbal note is not out of question.
I still belive that the best way is to say "I want so many holes of this kind, some of them may or may not terminate at certain features"
John,
I said many times, I have nothing against good machinists. Even best of them would like to know if the hole "may" or "should" cross another hole. There is a difference and it's good to specify it on the drawing.
Everybody,
Apparently the idea of "functional requirement" can be abandoned at the drop of a hat if it doesn't meet one's agenda. I have a theory about that.

 

[JNieman]

CH- I tried to emphasize 'design intent' because that will dictate the case-by-case scenario. In the OP, it appears the intent is that it does break through to the bore. So I addressed it as such, and applied the nomenclature that appears to suit the design intent "THRU TO BORE" as that is often the function required.

If it's not, a different note can be used as you specify. I'm not saying any which way is the "be-all end-all" just that "THRU TO BORE" does not, in any way, make a machinists job harder, and if that is the correct designation to get an accurately made part, true to design intent, without over- or under-defining the part, then it is quite valid, logical, and intuitive.

It's interesting that you specify a desire to abstain from this "THRU TO BORE" as if it were specifying a process (it isn't) but you're willing to specify "DRILL MAX" in your alternative.

_________________________________________
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]

O, puh-lease!

The meaning of my phrase wil not change if you substitute "drill" with "hole"

By the way, as a machine shop guy you do know what "counter-bore", counter-sink" and "spot-face" are, do you?

 

[JNieman]

The point was that you were unnecessarily picking nits by suggesting that defining a hole as being through-to-another-feature was defining the process. I know that saying "DRILL" is not constraining, but imo, it's more constraining than "THRU TO BORE" type notes. I do not think -either- of those constrains the process.

The drawing is of the finished part. When finished (key phrase) the hole will be through to the other feature. The steps it goes are up to manufacturing discretion unless specifically constrained. Defining a feature as being through-to-another-feature does not so constrain it.

_________________________________________
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]

JNieman,
You are avoiding my questions, ignoring my explanations and simply cannot go of me typing in not the best choice of a word.
This is beginning to look more like personal attack, so I have no reason to continue.

 

[powerhound]

drawoh got it right in his first post. The section view tells it all. Specifying a depth wouldn't really do it since there is really no depth to measure as KENAT said. If for some reason a section view is out of the question then "THRU ONE WALL" is an option. It does not imply that a wall has to be there before the hole is drilled although that will likely be the case. It only means that when the part is checked, the hole will be thru one wall only.

This really doesn't have to be this difficult.

CH, I don't even think a machinist has to be really good to understand what the OP print means. Granted, there are exceptions. Believe me when I say I've dealt with some brilliant engineers as well as some total soup bones. It's unfortuante that discussion like this comes about because of those soup bone machinists who screw up something so simple yet blame the engineers for not being "clear" on the drawing. They make us all look bad.

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

 

[Belanger]

From CH:

JP, you are invited to speak to the machinist as well.

But my point is that you are assuming that it's a "machined" part! Why?
Are you saying that when I look at a drawing that contains the words "thru one wall" that I must think that it's a machined part.

I hope not...

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems