Manufacturing tolerances 2

[Parsnip]

I am hoping this isn't a question that has been answered since I have searced the forums with no success.
I am having to do some draughting using geometric tolerances but need to find information on the sorts of geometric tolerances (e.g. concentricity, perpedicularty etc) associated with manufacturing processes and materials.
As an example I need to specifiy concentricty between two surfaces of a tube machined to different diameters.
I am sure I have seen a table showing this but have no idea where or even if I was just dreaming it!!
Any help would be appreciated.
Thanks in advance

 

[savis]

Try this web link to a Volvo standard available on the web:

http://www.tech.volvo.se/standard/docs/50622e.pdf

Sean

 

[Parsnip]

Thanks, but as with most other information I have found this deals with the definition of the geometric tolerance types not what values can be achieved. For example, with concentricity what sort of tolerance can be readily achieved that will not cost a fortune but ensure a "better than normal" requirement.
Caroline

 

[diamondjim]

In many text books, they have
values associated with different
types of machining equipment.
Not only are values shown but also
surface finishes. It is up to you
do try to match this with the age
of your manufacturing machines.
Obviously, they get worse as they age
just like people. You might want to
check Machineries Handbook and other
drafting manuals that should point
you in the right direction. They
are size and diameter related.

 

[ENG101]

You may want to look at this site, in particular Figure 10.

http://www.engr.ku.edu/~rhale/ae510/websites_f02/Manufacturing-tolerances.pdf

One other point, you mentioned specifying concentricity between two surfaces. If you are specifying a relationship between surfaces, you should use runout or profile. The majority of times that concentricity is used, it is actually misused. Concentricity is the relationship between two axes, and it is very expensive to verify.

Imagine machining a perfect rod from a piece of hex stock. The axis of the round turned section is perfect relative to the axis of the hex in the chuck. If you put an indicator on the round stock, you will see no movement of the dial.
However, if you reverse the machined piece, hold the round section and have the hex sticking out of the chuck, the indicator will be all over the place even though the axes of the two surfaces are still perfectly concentric.

To properly measure concentricity, you have to establish the axis of each surface, and then measure the relationship between the two. Royal pain the butt. Good luck.

Glenn

 

[Parsnip]

Cheers for that esp. ENG101 Figurs 9 & 10 shows just the sort of thing I was looking for.
I have a feeling I am going to grow to hate geometric tolerancing!!
Regards
Caroline

 

[CanEngJohn]

Specifying tolerances per the process you think is going to be used is a VERY throny approach to drawing components. What you should do is spec out what the component needs to be functional.

For example if you are working on a stepped shaft which is to work in a gearbox that is running at 15000 rpm then I would say that you might want a concentricity of about 0.005 mm (0.0002&quot in order to reduce unbalanced loads in the gear box. Yes this would be expensive but it is better than killing someone. And yes this can be done.

Flip to the other end of the spectrum. Lets say you want a stepped ID of a tube in order to allow clearance for a mating press fit component which assembles farther down. In this case the concetricity might not be critical and you might spec out a 1 mm (0.0393&quot concentricity if at all.

I think the important approach here is - give me a spec that produces a functional component and I'll give you the process to meet it. While design for manufacturability (which is what I think you are trying to achieve/play with) considers equipment capabailities what most people forget is that this is a compromise between economical processes and functional requirements. Just because your process can hold 0.01 mm conc doesn't mean your part needs to be spec'ed out that way. And conversely just because your process can only hold 0.5 mm doesn't mean your part should be dimensioned that way if it needs tighter.

 

[mrainey]

CanEngJohn,

Right on!