Drawing nomenclature

FredC · Feb 11, 2021

I have been making parts to drawings for 40+ years and still do not have a clear understanding of these 3 terms I see on drawings. Sometimes these dimensions are under my control and sometimes they are the result of the tolerances on purchased items.

Nominal: the drawing in hand has this for an assembly of 4 pcs with all the pcs having one or two dimensions affecting the assembled length.

Reference: one drawing in hand calls for facing off .117 the end of an Allen screw (5/8 Allen head) with a Machinery's handbook minimum depth of .307 and coming up with a ".3 Reference depth". If the starting dimension was minimal I could end up with an effective .190 depth.
4GSR this is one of your drawings.
Another drawing in hand has this for am assembled length of 2 pcs with 3 dimensions affecting the final result.

Typical: I have always taken this as a target dimension you would like to get but not always achievable. Maybe an average of purchased items?

BoxcarPete · Feb 11, 2021

If the drawings are made properly, those terms should mean this:

Nominal: the theoretically perfect geometry.

Reference: a dimension without a tolerance. It is listed to give information (e.g. an overall length when starting from a dowel pin zero) without forcing the machinist to math it out.

Typical: whenever you see a feature like the one dimensioned, an internal or external radius, chamfer, etc. make it like the one dimensioned.

FredC · Feb 11, 2021

BoxcarPete said:
If the drawings are made properly, those terms should mean this:

Nominal: the theoretically perfect geometry. (composite of the 4 pcs if each one is in the middle of the tolerance?)

Reference: a dimension without a tolerance. It is listed to give information (e.g. an overall length when starting from a dowel pin zero) without forcing the machinist to math it out.

Typical: whenever you see a feature like the one dimensioned, an internal or external radius, chamfer, etc. make it like the one dimensioned.

I kind of hope 4GSR sees this as his drawing is the biggest puzzle right now. The .3 reference is close to the starting minimum depth before I face .117 off the end. Not even close when I finish. Seems like a reference dimension should not change during machining. This drawing does not have any of the starting dimension of the purchased screws except for maybe this .3 Reference (.307 minimum).
BCPete, I was still editing when you replied, not sure if that changes anything.

4GSR · Feb 11, 2021

OMG!!!! I have made 100's of these in my shop over the years. It's not that critical on the depth of the hex socket. Get it within +/-.010" and machine the rest to the dimensions on the print. First operation, chuck up on the threads with soft jaws, turn the OD of the head of the flathead screw to drawing dimension of .672/.656". Face off the head to get the .17 depth. Next, cut the 82 degree bevel to 45 degrees and cut the thread relief to .480 dia.. This is all done in one operation. Remove from chuck. Bore out a set of soft jaws to hold the head of the screw so the other end can be finished. Cut to length, do counterturn. Counter turn OD is not that critical in diameter. The .450 length is critical. Hold as close as you can within +/-.005".

Not sure who you are doing this for, you need them to supply the slip stop ring so you can install them and check the stand off to make sure it is correct. I rather not post drawings here of all of this here. I know what I said is clear as mud. I'll try to post something shortly of how all this works. Ken

Edit: Added pictures to post.

The second view shows a gage used to control the depth of the counterbore in the part. This is where the J-pin goes. Ken

Oh, the .3 is the .307 as given from the standard.

4GSR · Feb 11, 2021

This drawing shows the profile of the screw used.

I just thought about something. I think your talking about the other screw that is made from a socket head cap screw. Let me dig it up and post comments about it. Ken

4GSR · Feb 11, 2021

Here's the other pin I'm thinking about. Ken

FredC · Feb 11, 2021

4GSR, I emailed the buyer and he said the depth of the Allen socket is not critical. When you make a drawing with that reference notation were you referring to before or after facing?
Without mentioning the customer's name or breaching confidentiality I can give you the date and part number on the drawing when I get back to the shop tomorrow. Maybe seeing the drawing in question will remind you of the intention. This was on a 5/8 Allen head cap screw with a head thickness of .620 nominal. Instructions say minimal cleanup on the inside and face the outside (hex side) to .5 thickness. I would assume the minimal cleanup on the inside is to preserve as much of the hard case as possible for wear resistance.
When I have made these for another customer, I used an over long screw, turned the features then cut it off so everything is done in one operation. I have got buckets full of slugs that I wanted to sell or give to a welder to use, so far no one can find a use for them. Used to have some good Manchester cut off inserts that would last for 100s of pcs. Ordered some Hertels that are supposed to be the same substrate and coating. We shall see.

OK, I re read your first post and the .3 was referring to before (.307 minimum), that is the answer I was looking for. So that was the only reference to any of the features of the purchased screw. This particular finished screw has no angles except small (.030) chamfers.

4GSR · Feb 11, 2021

If you can get me a part/drawing number I may know who it is for. I have supplied that drawing to three companies up in the DFW area over the years. I'm sure by now it's in other peoples hands, too. There are no secrets to this part. It is a very common part to those who use it in their tools they sell. Ken

FredC · Feb 11, 2021

4GSR said:
If you can get me a part/drawing number I may know who it is for. I have supplied that drawing to three companies up in the DFW area over the years. I'm sure by now it's in other peoples hands, too. There are no secrets to this part. It is a very common part to those who use it in their tools they sell. Ken

Yeah, I know this is pretty common stuff. the 2 drawings I have for this part are just a few thousands different. I do take the non disclosure agreements seriously. One of them said his drawing was the same as the competitor's. I only told him they were not the same. He looked at his requirements and did modify that drawing. they still were a little different, but the modified part worked as they ordered them again.

The other one sent me an out dated drawing 2 times in a row and did not catch it. Before it was all over they had about 20,000 pcs in stock that were wrong and had to be modified. I did post video on shortening those shear pins.

EmGo · Feb 11, 2021

FredC said:
Used to have some good Manchester cut off inserts that would last for 100s of pcs.

The oooonly way to fly, best in the west

Ordered some Hertels that are supposed to be the same substrate and coating. We shall see.

Please do .... I'm pissed that there is no more Manchester. Iscar, Sandvik, et al suck balls in comparison.

UncleFrank · Feb 12, 2021

Don't know it this helps you but in aircraft design:

Nominal (Nom.) - Theoretical perfect dimn ignoring tolerance or tolerance buildup.

Reference (Ref.) - A dimn/callout given in a subsequent view/sheet already specified in a previous view/sheet. However, parts must be final inspected to an original, not ref, dimn.

Typical (Typ.) - A dimn/callout given that also applies to similar part features in subsequent views/sheets unless otherwise specified.

75sv1 · Feb 12, 2021

UncleFrank said:
Don't know it this helps you but in aircraft design:

Nominal (Nom.) - Theoretical perfect dimn ignoring tolerance or tolerance buildup.

Reference (Ref.) - A dimn/callout given in a subsequent view/sheet already specified in a previous view/sheet. However, parts must be final inspected to an original, not ref, dimn.

Typical (Typ.) - A dimn/callout given that also applies to similar part features in subsequent views/sheets unless otherwise specified.

Ref. can also be a spec from another drawing. Take a casting drawing. Some of the pickup dimensions would be used for initial pickup. Also, used in assembly drawings, is needed to locate parts.

CORONA VIRUS · Feb 12, 2021

BoxcarPete said:
If the drawings are made properly, those terms should mean this:

Nominal: the theoretically perfect geometry.

Reference: a dimension without a tolerance. It is listed to give information (e.g. an overall length when starting from a dowel pin zero) without forcing the machinist to math it out.

Typical: whenever you see a feature like the one dimensioned, an internal or external radius, chamfer, etc. make it like the one dimensioned.

Nominal should be reworded. Nominal is the print dimension regardless of tolerance. If your print says 1.000" +.01/+.02, the nominal dimension is NOT 1.015. It is 1.000". Many people do not understand the correct definition of nominal.
Reference is NOT a dimension without tolerance. Reference is a dimension that is defined elsewhere on the print or feature standard, like a thread dimension.
BASIC is a dimension without a specified tolerance.

TeachMePlease · Feb 12, 2021

CORONA VIRUS said:
Nominal should be reworded. Nominal is the print dimension regardless of tolerance. If your print says 1.000" +.01/+.02, the nominal dimension is NOT 1.015. It is 1.000". Many people do not understand the correct definition of nominal.
Reference is NOT a dimension without tolerance. Reference is a dimension that is defined elsewhere on the print or feature standard, like a thread dimension.
BASIC is a dimension without a specified tolerance.

The number of arguments I've had with people about nominal vs mean....

BoxcarPete · Feb 12, 2021

CORONA VIRUS said:
Nominal should be reworded. Nominal is the print dimension regardless of tolerance. If your print says 1.000" +.01/+.02, the nominal dimension is NOT 1.015. It is 1.000". Many people do not understand the correct definition of nominal.
Reference is NOT a dimension without tolerance. Reference is a dimension that is defined elsewhere on the print or feature standard, like a thread dimension.
BASIC is a dimension without a specified tolerance.

That's not quite true. A basic dimension denotes the nominal size, but the tolerance for that dimension is carried elsewhere in a geometric control box rather than on the dimension itself. A reference dimension on the other hand, is information about a feature of size for informational purposes only, that is, there is NO tolerance associated with that dimension whatsoever. I mentioned one example of an overall length where a part has a zero point on another feature like a dowel pin (controlling features are distance from the pin in either direction), and others have given other legitimate uses for reference dimensions as well. But the fact is that it is simply information to be given for a machinist's reference and not a controlling feature, therefore no tolerance is associated with it. A basic dimension has an associated tolerance, but it's not on the dimension itself.

I'm not sure how you and I think nominal is any different. The theoretically perfect geometry IS what is on the print, the tolerances are the maximum allowable deviations from that perfect geometry. Unilateral or asymmetrical tolerances don't change that so I don't believe we disagree on that point whatsoever.

4GSR · Feb 12, 2021

I do not use "nominal" or "basic" on any of my drawings that I do for all the reasons just mentioned. I cannot stand argument from anyone on it's definitions and how to use it. Not that I don't know how to use it, it's more of it's definition out on the shop floor. It creates argument out on the shop floor, period!
Reference to me is just that, it is reference, and is not a controlling dimension at final inspection, period!

Okay guys, let's go back to work.

Ken

FredC · Feb 12, 2021

4GSR,
Particulars of the drawing were sent by PM email. Never used PM Email before but it seemed to work. All said and done I think I would have said "Reference before facing" to avoid confusion or otherwise made it clear this .3 was from industry specs for a 5/8 Allen head cap screw Before modifying.

On the drawing that mentioned Nominal, I was sent a factory drawing from an OEM that was using the same part and has an agreement with the originator of the drawing to use their final assembly drawing. Hope that was clear. WE make 3 of the 5 pcs that go into this assembly. Since we only have the final assembly drawing we have adjusted tolerances on the 3 pcs we make so finished length come out plus or minus .001" of the drawing nominal.

For every one else thanks for the input.

Some J Bolts finished and a few blanks for other styles. The finished ones are for the original customer.

CORONA VIRUS · Feb 12, 2021

BoxcarPete said:
That's not quite true. A basic dimension denotes the nominal size, but the tolerance for that dimension is carried elsewhere in a geometric control box rather than on the dimension itself. A reference dimension on the other hand, is information about a feature of size for informational purposes only, that is, there is NO tolerance associated with that dimension whatsoever. I mentioned one example of an overall length where a part has a zero point on another feature like a dowel pin (controlling features are distance from the pin in either direction), and others have given other legitimate uses for reference dimensions as well. But the fact is that it is simply information to be given for a machinist's reference and not a controlling feature, therefore no tolerance is associated with it. A basic dimension has an associated tolerance, but it's not on the dimension itself.

I'm not sure how you and I think nominal is any different. The theoretically perfect geometry IS what is on the print, the tolerances are the maximum allowable deviations from that perfect geometry. Unilateral or asymmetrical tolerances don't change that so I don't believe we disagree on that point whatsoever.

You are wrong. The basic dimension has no tolerance. It is drawn inside a rectangle. It is a standard feature on Tool and Die prints. It is what we call an inspector's dimension. A reference dimension is a dimensioned somewhere else. Commonly it is depicted when the reference dimension is obtained by adding multiple dimensions to get to the reference dimension. Or, if that dimension is in another print location and is being REFERENCED for ease of viewing. THAT is why they call it reference.
"The theoretically perfect geometry" ...perfect for whom? The engineer, or the machinist. Perfect geometries often do not work for either. For example, an engineer draws a 1 inch shaft (not making fun of you). Then he makes a 1 inch hole. Instead of taking the time (laziness)to make more geometry he uses the same circle to draw both the shaft and the hole. Then he either applies a tolerance to make the hole bigger, the shaft smaller or both. In either case, your "perfect dimension" will not allow the 2 parts to fit together without force. So, they are not perfect.

boslab · Feb 12, 2021

I’ve used reference on a drawing but tried to avoid lassoing it round dimensions with tolerance, sometimes there was a capital M in a circle after
(Maximum material condition, or at least it was years ago)
Mark

UncleFrank · Feb 13, 2021

75sv1 said:
Ref. can also be a spec from another drawing. Take a casting drawing. Some of the pickup dimensions would be used for initial pickup. Also, used in assembly drawings, is needed to locate parts.

True as Ref. could refer to other separate dwgs/lofts/specs/etc but those Ref.'s must have the other separate dwg/loft/spec/etc number listed in the note. I was trying to describe a Ref. dimn/callout limited to just one specific dwg.

Drawing nomenclature

Diamond

Stainless

Diamond

Diamond

Attachments

Diamond

Attachments

Diamond

Attachments

Diamond

Diamond

Diamond

Diamond

Cast Iron

Hot Rolled

Banned

Diamond

Stainless

Diamond

Diamond

Banned

Titanium

Cast Iron

Similar threads