Drawing Philosophies (help!) 2

[evolDiesel]

Please look at the attached print and tell me if this is legal, and if so, legal by what standard (ASME Y14.100-2004 is what we use).

This part has a locating fixture for a jig (see right hand view)... after locating it, we face it off (see left hand view).

These have been 2 different part numbers... when the left one is built off the right one.

Recently I had an engineer come to me and suggest we could put both of these on one print using configurations (SWx) ... just as you see in the attached print.

What do you guys think of putting these 2 parts on one print? What is the official rule on having some views on a print not match up with other views (some of these views would not have the facing operation). Seems confusign to me.

 

[KENAT]

Are you talking about using "dash" numbers. This is often used for either left & right hand parts and for items that are basically similar but maybe there are several different lengths, Y14.24-1999 has an example (fig 5) of a 'tabulated monodetail drawing. It also talks about left/right hand (not in those terms) in section 3 (mainly a foot note).

However, it apears your left & right aren't just mirror images, that one has an extra feature (or lack there of) so I'd be cautious.

A good philosophy is "Just because the CAD software lets you do it doesn't make it right".

KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

OK, I re-read your post and actually you aren't talking about quite what I thought you were.

I'm not sure I understand why you don't just have the finished part detailed. I think I'd lean toward separate numbers as I certainly think your single drawing might be confusing.

KENAT, probably the least qualified checker you'll ever meet...

 

[evolDiesel]

I know what you're talking about.

I will clarify that this is not an application of length or handedness.

This example here shows a part that has undergone initial operations (view on the right)... then it either gets stocked or transported to a different machine to get the final operation (view on the left). That's why we will have multiple part numbers and prints to reflect the life of this part as it makes it's way to a "finished" part.

I just don't like the idea of having a view of a part that doesn't match the other views. It's confusing for inspection... or even for manufacturing the part (if I had to read and interpret this print).

Thanks for your response KENAT

 

[evolDiesel]

KENAT - In a perfect world we would have one part number and one finished part, unfortunately, we have different machines, different operations, stock needs... that force us to create multiple level parts that look like this:

A = Unfinished (material is raw)
B = Semifinished (material is "A")
C = Finished (material is "B")

Does that clarify? Thanks again

 

[KENAT]

I've seen similar done once or twice but it never seemed very efficient etc. but you probably know what suits your needs better than I.

So you definitely need separate part numbers because of the stocking issue.

The question is whether you can have the different part numbers detailed on the same drawing then.

You're effectively talking about a Multidetail drawing per section 3.2 of ASME Y14.24-1999. Figure 6 is an example though I'm not clear how they identify which part is which number in that example. The standard does caution against doing this unless you're sure the benefits outweigh the problems.

I suggest you take a look at 14.24, maybe some posters that have used these more than I can comment.


KENAT, probably the least qualified checker you'll ever meet...

 

[ewh]

The only place we use dash numbers is for tooling assemblies. Each component is detailed on the same drawing and has its own dash number. The completed assembly is the part number without a dash number. I would caution against using dash numbers as you have described; it will probably cause more confusion than it's worth due to the mixture of operations involved.

When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]

 

[ctopher]

I always have separate part numbers and drawings for parts.
But, for tooling/fixtures the parts that make up the tool are all stamped with the same tool number. Therefore, I create multiple sheets and add all parts as dash numbers. When I created military/aerospace designs, this was a requirement for us.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[fcsuper]

Sounds like you need a make-from drawing. I suggest that the items should be two different part numbers, each on their own drawing. Configurations with SW models is fine, but don't use one drawing for both configurations if they are really different parts. Just some thoughts.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[evolDiesel]

Anything having to with "dash numbers" or anything more sophisticated than "dumb numbers" won't work with us and our part number philosophy (everything is given a dumb 6 digit number).

So, none of those are options

Multiple drawing sheets gets a little scary (if it's for different parts). In other words, I wouldn't want to bury unique parts inside other sheets of a drawing.

Is it just me, or is "one part.. one drawing" out of date? I always thought that philosophy was very robust and prudent

 

[evolDiesel]

Also - I've looked thru the ASME standard and I'm not having any luck locating a defitive answer to my question (via a standard such as the ASME standard).

Are you guys aware of drawing standard that discusses multiple parts on a single print?

 

[drawoh]

evolDiesel,

My thoughts are...
[ol]
[li]Is there any need to document the flange without the face? I, personally, do not care how the fabricator arrives at the final, faced part. If your angle cut is a datum, the shop must fabricate it first, and use to to fixture for facing. If he is dumb enough that you have to explain this to him, your problem is not drafting standards.[/li]
[li]Would you fabricate a batch of unfaced parts and place them in stock? In that case, you need a separate part number so that they can be separated from the faced parts. This gives you the option of having more than one face dimension, each of which requires its own unique part number.[/li]
[/ol]

JHG

 

[KENAT]

evolDiesel ASME Y14.24-1999 section 3.2 Multi Detail Drawings. is the ASME reference.

However, now that you've said dash numbers aren't an option I'd lean toward keeping completely separate drawings as well as part numbers.

As you mention, one will be a 'make from' the other.

KENAT, probably the least qualified checker you'll ever meet...

 

[vigildesign]

We often have this type of drawing with two model configurations, for different machining processes. In house work only. The difference in features is not as great as the image shown, but a note is used similar to this:

MANUFACTURE OF THIS PART REQUIRES TWO MACHINING STAGES. (A) STANDARD MACHINING AND (B) DIAMOND MACHINING. SHEET 1 DEFINES STAGE (A). SHEET 2 DEFINES STAGE (B).

Marcelino Vigil
GDTP T-0377
CSWP

 

[ewh]

I agree with KENAT. Two numbers and two drawings would be better.
drawoh has an excellent suggestion, one that we are implementing more. That is to create a "reduced dimension drawing" defining the finished part, and leave the non-critical details to the fabricator. This is assuming that the fabricator can interrogate the model for information not on the drawing.

When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]

 

[ctopher]

I agree, separate parts, separate drawings. the drawings show the final configuration...without processes.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[evolDiesel]

LOL... I live in a different world.

All our prints must be created such that they are all the information required to build the part; whether it be in-house or out-of-house.

Our situation is so sterile that a design engineer (me) doesn't have any social interation at all w/ the machinist/fabricator.

And all they have access to is this hard copy print (no digital model to pull dimensions from).

 

[evolDiesel]

ctopher,

We have a CAD Admin guy who's mantra is "you can't dictate processes on a drawing" and he says he got it from DOD standards.

I tend to agree that you at least have to be careful on how far you go defining processes (unless it's an assembly instruction print that's whole intent is to describe processes).

If we put these 2 parts on a print we necessarily must describe a process... in the very least... to establish that one part makes the other, and not the other way around.

Good point.

 

[ctopher]

You can have "make from" on a print. Assembly instructions should be on a separate doc, plating/machining/etc processes should be called out in a note via its spec number.
Although there are standards and specs, most companies do it how they want to do it anyway.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[KENAT]

First part, 000001 for instance, is the initial part.

Second part, 000002 for instance, is made by modifying part 000001. On drawing for 000002 the Material box in the format for material you say 000001 (depending on your convention it may need to be a note and you may need to spellout "MAKE FROM PART NUMBER 000001". This isn't really describing a process as I'd see it.

If you tried to do both on the same print you'd have in effect do the same, but I'm really not sure putting it on one print is a good idea from what you say.

As to not normally dictating process on the drawing this is from ASME Y14.5M-1994 section 1.4 FUNDAMENTAL RULES (e).

KENAT, probably the least qualified checker you'll ever meet...