relative machining costs as related to dimensioning style 1

[aon1]

Is there any information out there, quick reference tool of relative machining costs related to dimensioning style?

i.e.
1) dimension style: fractional; suggests a metal scale or measuring tape used = +/- 1/32" accuracy is adequate and means less care required, less cost.

2) dimension style: decimal; requires an instrument (vernier) to check; number of decimal places requires more care and possibly different machine to achieve, incrementally more cost.

 

[tomwalz]

I think of fractions as being used to measure wood in secondary wood manufacturing and metal being measured in decimals.

Fractions are nominal and you don't build anything using them. E.G. If we buy a carbide saw tip 3/8" long it will be minus zero and plus as much as 0.007". We buy a 3/8" tip but put it on a saw and grind it to plus or minus 0.0005".

A lot of wood is measured with verniers.

Off the top of my head I would say the cost goes up exponentially with each additional place to the right of the decimal point. That’s probably not right but it gets the idea across.

If you can make a saw cut (kerf) 0.001” thinner it can be worth as much as $50,000 a year to a saw mill.

Darned interesting question.

We are in several industries and it changes from one to another. Engineers use it differently than mechanics and R&D engineers tend to use it yet another way.

Remember that all communication is maybe 25% good. With repeated effort and precise drawings you might hit 90% good.


Thomas J. Walz
Carbide Processors, Inc.

http://www.carbideprocessors.com

 

[unclesyd]

One of the first lessons I learned about machining was that 0's to right of the decimal point cost money and as tomwalz states it is almost exponential though not as steep a curve as it was before the advent of NC machines. We have a very large shop building where there is fabrication shop on one end and a sheet metal shop on the other with a machine shop in the middle. The fab shop and sheet metal shop work with fractions while the machine shop is 98% decimal, the main exception is the call out for the starting material stock and tooling.
It is all too easy to add places to the right of the decimal just to imply the need for precision. This leads to all types of additional cost not only from the machining standpoint but from the quality control. Typically to check a 0.00X callout you have to be able to check to 0.000X. When you get into 0.000X dimensions you have to start looking at shop temperature control. Then then is the worry how the end user will verify the part.

Even when using fractions don't callout a 1/32" for something like vessel and pipe fabrication where even 1/16" is tight dimension, especially for older welders and fitters. A 1/32" callout could be OK for the sheet metal shop on small size jobs but generally not necessary.

There are a few other traps in calling out in dimensioning process no matter the precision. One is that the dimensions can start getting stacked or interdependent so each new machining operation requires more precision. This leads to problems with position/reposition of the part being machined. Every time a part being machined has to be repositioned costs money, especially as the precision goes up.

Always look at the end use of component/part and what the capabilities of the shop that will make it and go with that. If you require a greater precison than a shop normally works in look else where.

 

[BowTied]

I am not aware of a book or convention that covers what you are asking. I do expect a tape measure to be used when I specify fractions, but I then keep in mind that it is not practical to expect accurate measurements if I specify ±1/64" - I stick 1/16ths typically.

To build on what unclesyd says - use of datum dimensionsing instead of chain dimensioning where possible is desriable. This ensures each feature can have the largest tolerance possible and can avoid additive tolereance stack-up which can have parts not fitting together at assembly without large clearances.

To me dimension accuracy and tolerance dictates cost simply because it also dictates the manufacturing process to some extent. ie You can cut something on a band saw that is ±1/16" or ±.06" but ±.006" requires a more precise tool = $$ of course.

I find fractions useful in certain places, places like for weld sizes especially if the welding is done by hand. A 1/8" fillet weld is more meaningful to a welder than a .125" fillet weld. Also for assembly where a component must be positioned in a certain range.

If you have particular needs to fulfil and the drawing tolerance block is insufficient to capture this I suggest creating a specification that is referenced in drawing notes that a vendor must adhere to and covers your needs. Of if this is a QA issue, a similar guidleine can cover you.
Hope that helps.
Ron

 

[aon1]

Thank you all for your responses.

I was wondering how a machine shop might quantify an estimate in that this line of thought could be a useful reference tool to a designer ... where do we draw the line in specifying a tolerence ... something to aid in deciding how necessary a fine tolerence might really be.

I'm an olderer fella who had been taught by even older guys. My way (the common sense era?) seems to have given way to the techno-gizmo youth in that I'm told fractions are passe, decimals are the only proper method for dimensioning anything mechanical... Fractions = architectual style is for architects. I would have used what 'common sense' determined was most appropriate for the application be it a fraction or a decimal.

Am I alone with this train of thought?

 

[BowTied]

I think part of what you are experiencing is that computers "think" in decimals - and software, unless specially geared for an industry like Architecture, lives in decimals. Mechanical CAD packages have been primarily set-up in decimal form, though there are exceptions.

This issue is doubled if the person in question was raised primarily on the Metric system where base 10 counting is so easy - thinking in fractions would then seem very old school for sure.

"common sense era". I like that....Trouble is, common sense ain't so common anymore.

 

[arunmrao]

Very good tips from unclesyd and tom. I have always understood that civil constructions use tape measurements,while all other mechanical engineering activities use verniers.

With the advent of computers a lot of design data generated have several decimals,but physically these numbers might not have any significance. Be careful not to fall into this trap.



Chocolates,men,coffee: are somethings liked better rich!!
(noticed in a coffee shop)

 

[mrainey]

There's a lot of inconsistency out there about decimal places vs default tolerances - some companies specify +-.010 with a three place decimal, others +-.003, most seem to go with +-.005. Some allow +-1/64 with a fractional dimension, others +-1/32.

When a closer tolerance is required for a specific dimension, it's spelled out.

Speaking as a manufacturing engineer with a focus on CNC machining, all that really mattered to me were tolerances.

I learned early in the game that making assumptions about blueprint conventions is a very bad idea. Study every dimension, think about every tolerance.



Software For Metalworking

http://closetolerancesoftware.com

 

[KENAT]

It will depend what tolerances are invoked by the drawing.

It's wrong to assume fractional dimensions have one level of precision while decimal have another without looking what the drawing actually says about tolerance.

Unless the drawing itself, or a standard referenced by the drawing states what the tolerance is then you don't have that information.

Which would be cheaper, a part all in fractions with a block tolerance of +- 1/128 or a part in decimals with a block tolerance of +-.030?

It is the tolerance that should drive cost not whether it's shown in decimals or fractions.

However, because many are ignorant of this the fractionally dimensioned part may actually come back with a cheaper quote.

aon. The current industry standard for dimensioning & tolerancing (at least in the US) only address decimals, not fractions.

Ask this question in forum1103 and you'll likely get more explanation.

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

 

[aon1]

KENAT
Typically (but you are correct that it is not always) a drawing will have a default tolerance block to fab/mach to if no other tolerance is noted.

As I mention before I am from the end of an era when drafting as a "trade" was phasing out and... well here we are.

Back in the old days (when we walked to school up hill both ways ... sorry I could resist) fractions were quite common.

I understand Y14 does not even mention fractions as a dimension style. Seems a bit short sighted to this ol' fart.

Anyway I digress. My orginal question had to do with the exisitance of some type of factor upon which cost of machining versus tolerance might be based.

i.e if fractions were to be the base = x 1 cost
one decimal might be x 1.25 cost of fractional tolerance
two might be x 1.5 cost
etc...

I wonder how a machine shop estimates the cost of doing a job?

 

[KENAT]

aon, I still don't see that your question really makes sense. It's the tolerance itself that should drive the cost from this point of view. While the case has been made before this isn't entirly true in practice, especially if GD&T is used, in this case I'd have thought it applies.

So long as the same tolerance is invoked I don't see why using fractions or decimals should make a bit of difference to cost. Whether it's expressed as +-1/32 or +-.03 (approx) shouldn't make a difference.

I will admit that in most of the tolerance blocks I've seen with fractions still in them, the tolerance for dimensions expressed with fractionals is looser than for those expressed with decimals.

If you just want an answer based on how I think people would perceive the drawings without actually looking closely at the actual tolerance requirements then I'd expect the fractional to be cheaper.

However, I'd have second thoughts about using a shop that costed parts in that way.

As to determining what tolerance is applicable to a part, this should be primarily driven by function. If the tolerances you arrive at aren't achievable in a cost effective manner then you need to re-look at your design.

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

 

[mrainey]

You have to consider how the part will be machined.

Holding +-.001 on a turned diameter is normally pretty easy on a good CNC lathe. Holding +-.001 between two faces on the same workpiece, and on the same CNC lathe, might be trickier (more expensive) if the faces had to be machined in separate operations.

Software For Metalworking

http://closetolerancesoftware.com

 

[aon1]

I follow what you both are saying.

I've always understood that a closer tolerance required more attention and care resulting in more effort and drives cost up.

Maybe this line of thinking is wrong... however I know that some materials, shapes are trickery to get a close tolerance on because of simple thermodynamics... as you machine the part the action cause the part to heat up and expand making it more dificult to control the dimension.

Yes I know that is why they use cutting oils but depending on how fine you need to be they sometimes aren't enough on there own. Hence the need for more machining steps to reduce the thermal expansion and better control the finished dimension ... more labor = more cost.

I am beginning to accept that machine shops quoting a job is all by gut feel and experience.

 

[KENAT]

I guess my point can by summarized by this, when looking at the effect of tolerance on a part it's not primarily how the tolerance is expressed that should be driving the cost but what the tolerance is.

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

 

[tomwalz]

Dear aon1,

Sure it is gut feel and experience. What else is there?

When we quote the first thing we consider is the person. Do we like them? Do they know what they are doing? Will they listen to us?

We use our gut feel about the person and match it with our experience. I have done a lot of consulting over the years as well as a lot of contract R&D. I avoid that now. Now we like building things for folks that know what they want.

Experience has told us that everybody involved is happiest if there is a clear, simple straightforward set of directions.

I said earlier that communication is never perfect. We need someone who knows what they want well enough to answer questions about it.

Give us a set of plans and / or specs with tolerances exactly the way you want them. If we can’t match them we will tell you.

If you specify an outside dimension to three decimal places we will ask you about it and suggest ways you might save money.

I think your question has an answer but I think it is buried under more important factors.

I do not mean to be offensive but we would prefer not to work with someone who asked the sort of question you did to start this thread. Intellectually it is fun with my morning coffee and I thank you for it. Practically, we really like to build things. Tell us what you want and we will build it. If you want a half inch saw tip just tell us. We know they come 0.500” to 0.507” long. We will supply a saw blade ground to a nominal + / - 0.001” nominal and actually to a + / - 0.0004”. We like beating specifications. The better we grind the better you will like our saw blade.

If you asked for us to use saw tips that were ½” + / - 0.0004” we would politely explain that we don’t do that. It would show that you did not understand the manufacturing process and it would be a task we do not do regularly.

If you just want to buy tips precision ground it would turn a $0.25 item into a $4.00 item and you would pay for a lot of lost time.


Thomas J. Walz
Carbide Processors, Inc.

http://www.carbideprocessors.com

 

[aon1]

Tom

Thank you very much for the honest and brutal response!
(seriously!)

I was looking for a quick reference for designers to consider. Practically everyone has indicated there ain't one.

It is likely (as you pointed out) impossible with a one of design (R&D).

You have no idea how much this applies to us!

I thank you all once again and although I did not get the answer I was seeking I did find this forum very worthwhile.

Al.

 

[KENAT]

Maybe this'll help though it sounds like you probably know most of it already thread404-197410

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

 

[tomwalz]

I wasn’t going for brutal. Sorry.

I live in a world where clear, definitive answers are highly preferred. I really try for charming, settle for polite but sometimes get rude.

Besides, after reading several of your posts, I got the impression that you were very bright with a lot of experience and already had your own answers from both theoretical and practical considerations.

My favorite question is about how to find the volume of a mound of material when all you know is the height as well as the length and width of the base. I don’t know the answer and can’t find anyone who does but every now and again I ask just in case.

Tom

P.S. boy, were you correct about drafting / mechanical drawing.


Thomas J. Walz
Carbide Processors, Inc.

http://www.carbideprocessors.com