Dimensioning and tolerancing close fitting mating parts 1

[John2002]

Hello,

I have a question regarding the best way to dimension and tolerance close fitting, mating parts.

I have two parts made from 60-61-T6 aluminum that mate with a tongue and groove fit. I have a 0.250" wide tongue that must fit into a 0.250" wide groove. There cannot be any interference between the tongue and groove, but the parts should fit together with the least amount of clearance possible at the width.

Periodically, the part with the groove will slide on the part with the tongue very slowly, but the sliding is so intermittent and slow that friction and wear is not an issue.

I think the maximum amount of clearance I could get away with between the parts would be about .004" & I would feel more comfortable with .002".

1.which of the following dimension /tolerances would be best to keep clearance to a minimum (or are both the same)? They both have the same amount of total clearance possible, but from a machining standpoint, would one produce better overall results for the majority of parts?

A. Groove 0.250" wide +/- 0.001"
Tongue 0.249" wide + 0.000" -0.002"
Worst case = 0.004" clearance

B. Groove 0.250" wide + 0.002" -0.000"
Tongue 0.250" wide + 0.000" -0.002"
Worst case = 0.004" clearance

2. Are there any general guidelines when dimensioning and tolerancing mating parts like this? I want to eliminate as much clearance as possible and still keep costs reasonable. At what point would tolerances begin to really become a cost issue?

3.Provided the total variance in tolerance is the same, in general, is there any difference in machining cost between bilateral or unilateral tolerancing? For example, (plus or minus 0.001&quot versus (plus 0.000 minus .002&quot.

Thanks for your help. I would appreciate any feedback.

John

 

[diamondjim]

Our shop prefers bilateral tolerances.
It is only a mental set or habit that you
would prefer one to the other. I like
to think in max material condition for shaft
and min material for bores so I can quickly
determine min clearance. If you are making
mucho parts, you could match the clearances.
It will be fun to see other responses.

Often in Europe they will use the nominal
dimension with only plus tolerance on the
one part such as shaft or tong or key,
and two negative tolerances on the bore or notch
or keyway.

 

[MadMango]

1. Method B will hold your tolerances tighter than Method A. At MMC, you will have zero clearance. With Method A, you will have .002 clearance. At LMC, you will have .004 clearance, and with Method A you will have .001

2. You should invest in a copy of Machinery's Handbook, they have entire chapters devoted to this.

3. I think bilateral tolerancing would generate higher costs, since there isn't the same amount of "slop" avialable for the machinists. "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[tomwalz]

My first thought is that a lot of this depends on the size, shape, length, etc, of the parts.

Metal moves. It moves all the time. Out here in airplane country tolerances are sometimes specified at particular temperatures. Forged metal moves. Long shapes tend to sag. Material tends to have a grain and can twist.

I am talking about complex shaped, ten foot parts with of forged aluminum machined +/-0.001 to and +/- 0.0005".

Carbide saw tips are sized 0.150" -0, +.007 because it has to be a definite width. The extra gets ground off.

Tom

 

[charlie300]

The format does depend on how the machine shop likes to work. BiLateral (or equal tolerenced +/- dimensions) is what I like to give to prevent mental math on what the target is.

The real problem is that on paper, both conditions would be a bad design. You are not controlling the minimum clearance and could end up with a press fit in a shop where mating pieces were made by different people. Sure you could rework the pieces, but that is cost too.

Condition A with the tongue being .247 +/- .001 is what I would suggest. This would yeild the rare possibility of a .005 Maximum condition, but generate .001-.003 slip fit most often.

If you were serious about the uppper slip fit of .004", and did not want to tighten the tolerence (which could effect cost), you could take the unusual step of putting a note on both parts describing a maximum .004" was allowed and a slip fit of say .002" was prefered.

Charlie

 

[atlarson]

John,

The answer to your question depends on the method of manufacture of this device. If it is a low volume, high value item built on manually operated machines, then you could use unilateral tolerancing. A good machinist will then "sneak up" on your nominal dimensions by measuring his parts before taking his final cuts. If however, the parts are higher volume and will be manufactured using N.C. machines, I suggest that you use bilateral tolerancing. Although these machines can be extremely accurate, they generally should be programmed to a mean dimension so that process variables are least likely to produce bad parts.

Another consideration: If you design your tounge and grove to have zero clearance at the tolerance limits, you may actually end up with a slight interference fit between the parts. This could be due to measuring inaccuracies or not quite flat surfaces. You may want to design .001 or .0005 clearance between the parts at MMC.

Andy

 

[John2002]

Hello,

I just wanted to thank everyone for their replies to my post. Your comments were very interesting and helpful.

Sincerely,
John