Tight Tolerancing and Fabrication

[JLang17]

For practice I am applying GD&T to an assembly that has already been made. The design is filled with extremely tight fits (for example a fixed fastener dia of .112 with a clearance hole dia of .114). The positional tolerances I'm calculating have been from .0005 and up.

What throws me off is that this assembly has been fabricated based on these plans. Since the plans didn't have any GD&T at the time of fabrication, can I assume that many of these clearance holes were made larger? That the fabricators fudged the hole sizes to make everything work?

If I were to accept this and actually tolerance these things at .0005, or zero for that matter, would that even be possible? (putting cost aside).

 

[ctopher]

Are these tight tolerances used on the assembly for some hardware attachment, or for the parts themselves?

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08; CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[drawoh]

JLang17,

Have you inspected the parts and verified for example that the Ø.114" hole is indeed Ø.114"?

Were the parts fabricated separately, or were pieces drilled together?

JHG

 

[ajack1]

Surely that depends on how the parts are manufactured? If the holes are put in with one set up on a CNC mill or pierced on a press tool then it would not be unreasonable to expect them to be within those limits to each other.

 

[ringster]

I have always thought it was good design practice to provide the maximum allowable tolerances for parts. I would question what drives this design to such a tight tolerance. Not just a question of "is it achiievable".

 

[fcsuper]

Some engineers like to design assemblies so that the fasteners themselves do the alignment. In those cases, I've seen ridiculously tight tols on holes (often sqr tols, not even geotols). This should be avoided if the device even will need maintenance (which most do). It's poor practice to use threaded fasteners to align parts. This should be done with fits, grooves, and/or alignment pins.

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

 

[MotorVib]

The better question that you should ask is how hard is it to assembly. Go and ask the guy who is assembling and then inspect a few parts. In the end the guy who is doing the assembly is the one that is going to be living with the problems of the assembly.

Chris

"In this house, we obey the laws of thermodynamics." Homer Simpson

 

[aardvarkdw]

The parts might meet spec but the assembler may be filing out the holes so that things fit without you knowing it. He wont say anything without you asking because he's got to deburr anyway and besides he is getting paid by the hour...

David

 

[JLang17]

Thanks for the replies, the designer will be in next week so I have a few things to discuss with him. I'm not sure if I'll be able to dis-assemble the device to inspect, but I'm sure he'll have some insightful feedback.

 

[drawoh]

JLang17,

You also want to talk to the guy who built it. The designer may be surprised at how it actually got fabricated and assembled.

JHG

 

[SDETERS]

Do tolerance stack to double check your dims and tolerances. If you do proper tolerance stacks then this makes sure your assembly will go together

 

[desertfox]

Hi JLang17

If the clearance holes for the fasteners are as tight as you say and the fabrication went together without problems then you can assume that the components were made within the tolerances you have calculated.
However 0.002" seems a very tight tolerance for a conventional fastener unless it was a special fastener like a shoulder bolt for instance.
While your practising the G&T consider the following things like what machining process or fabrication process did the components under go and are those processes capable of providing the accuracy the parts are toleranced too.
More importantly look at the function of the fabrication and decide whether it needs such tight tolerancing or not.
The basis of any design should take account of fit and function and not just how accurate something can be made.
Tolerance stacks are also very important and if you start with a very tight tolerance you will find that once you are assembling more than several components your tolerancing tends to get tighter and tighter to ensure parts can fit together, so try to give a tolerances as large as possible within the fit and function for the part, that way you will have a good design without excessive and unnecessary cost.

regards

desertfox

 

[ringster]

desertfox,

I dont believe that tolerances should ever be assumed to be correct. THEY NEED TO BE VERIFIED by ISPECTION.

The fact that 2 parts happen to fit together, by itsself, does not assure interchangeability for future replacement of parts.

Interchangeability if one of the benefits of using GD and T as I recall from years ago.

 

[desertfox]

hi Ringster

Well if you can never assume your dimensions and tolerances are correct you can't do tolerance stacks prior to manufacture, at some point in time you have to assume tolerances and dimensions are correct to at least check a new design.
Inspection I agree is required to establish whether or not the part is within tolerance once its been made, however prior to the above fabrication being assembled it is usual for parts to be individually inspected for dimensional correctness, so I assume that the individual parts that make this assembly have been inspected already reading the original post. In addition I also stated that if the assembly was made without problems (ie manufacturing errors)then it is reasonable to assume that the dimensions and tolerances are correct.

regards

desertfox

 

[KENAT]

Jlang, welcome to my world.

I (and my contract colleagues) frequently get asked to check drawings that have already had components made from them which 'worked' but a quick tolerance analysis of will reveal potentially large interferences. Sometimes it's prototype batches but sometimes its items that have been in production for some time.

Philosophy here seems to be, if you can build one prototype and it fits together then you're good to go no need to bother about tolerances before or after. This bites us in the a$$ every now and then. It's especially bad if we change machine shops or maybe split mating parts originally made at one shop across several, or sometimes if we have changes in our own assembly staff etc.

You haven't mentioned what the tolerance on the hole size is, you only explicitly talk about position. Typical drill tolerances tend to be -.001 +.004 (or more on the + as the drill size increases)

http://www.engineersedge.com/drill_sizes.htm.

So, unless you specify tighter on your prints your .114 will likely be drilled by a 2.9mm drill (.1142) with tolerance of -.001 +.004. This means that it's likely that most of your clearance holes are oversized. This in turn buys you something on location - even if the old prints didn't explicitly mention MMC a larger hole at least accommodates more movement of the threaded hole.

Second, the thread value you give of .112 is a max, so in practice will usually be smaller than that, which again will help with fit.

So, even without exceeding the (assumed) stated tolerance you at least statistically have a better chance of fit.

Then as others hint at, you have the person putting it together. Even if they aren’t deliberately filing, reaming or otherwise enlarging the clearance holes, they may do so by forcing the screws in ‘chewing’ out the side of the hole, especially if the part with the clearance hole is thin and/or of softer material than the screws.

.0005 position on a non threaded hole is achievable, may not be cheap, but we have parts with that kind of tolerance, and tight hole size tolerance. However, these are mostly on precision pin location holes etc not for matching threaded holes. 0 position is legitimate if you invoke MMC.

On threaded holes I would not expect .0005 to be realistically achievable for reasonable cost. I have experienced colleagues who refuse to put less than .005 position for threaded holes and prefer at least .010.

I had some parts similar to yours where I had to make an updated threaded hole pattern (#4 I think) work with existing clearance holes. Based on the calculations I needed 0, or maybe slight negative (which is impossible) position on the threaded holes. I spoke to the machine shop, and bear in mind this was a precision part used on microscopes so the shop is used to tight tolerances, and the tightest they’d commit to was .003 positional on the threaded holes.

So in this case I was not able to guarantee fit at worst case, but did my best to minimize the chances of interference and relied on the factors above to ensure fit most of the time.

Simplistically conventional hole pattern calculations (as in ASME Y14.5M –1994 appendix B) assume worst case, in practice worst case is rarely achieved with actual parts so the parts go together much of the time. The problem of course occurs when they don’t.


KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

 

[drawoh]

KENAT,

You make an intertesting point about parts going to the same machine shop. Machine shops look at drawings, and often recognize pieces that have to be assembled. I know some designers that send their assembly drawings out with their fabrication drawings, to help the machinists along with this.

Personally, I regard my assembly drawings and parts lists as proprietary. I do not want to send them out. I am quite capable of doing properly toleranced, GD&T drawings.

Ask yourself how a machinist goes about making parts fit. He does not want you to complain about his stuff. His pride and reputation are on the line.

The machining process is forgiving of crappy drafting. That does not mean the crappy drafter is safe when the drawings go out to sheet metal shops, welders and foundries. It does not mean the machinists are not making smart-ass remarks about us, behind our backs.

JHG

 

[KENAT]

drawoh, in our case it's also the fact that we have (at least historically) a close relationship with at least one 'precision' machine shop. So most of their stuff comes in close to nominal, they rarely approach the limits, not sure if it's just that they're that precise or if they know most of our prints aren't properly toleranced and compensate. I do know they have their own redlined prints etc for some parts.

We are starting to shop around more to find lower costs and its here that incomplete and/or poorly toleranced prints, even of things we've been making for years, are biting us.


KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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