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

 

[sprintcar]

You need to use some GD&T on this - max and min material conditions with Profile should narrow it down.
It also depends on mfg process - extruded or machined.
Keep in mind that temperature plays a role, so you might want to spec the inspection temperature and check your clearances at operating temps.
enjoy Keep the wheels on the ground
Bob
showshine@aol.com

 

[gearguru]

The ISO system of fits (metric) is the tool for situations like this. You can try it - convert your dimensions in mm, find appropriate internal/external part combination of fits (like 12.7H7/f6), check for the numerical values and convert it back in inches (if necessary). The ISO fits and the charts with their numerical values are also in Machinery's handbook.
gearguru

 

[iaguy]

Part of you question asks do you use .250 +/- .001 or .250 +.002/-.000. The answer to that is in your tooling. if you have a cutter for the slot that is .250 then you would use .250 +/-.001. This allows for over size cutting in the slot and wear on the tool. If you cutter is .251 then you use .250 +.002/-.000 same as above. Your toleance is the same. Your Base dimension is a function of the cutting tool.

Lynn

 

[jjjaos]

I agree that your groove width is a function of your cutting tool. I recommend that you go with a +.002/-.000 slot width. Milling cutters and end mills tend to cut over their nominal size due to runout. Furthermore, according to the Machinery's Handbook, standard keyway tolerances are +.002/-.000 and +.000/-.002 for the key. I think this application is similar to cutting keyways.

 

[PrecisionMachining]

Depending on the length of the part, they can even be Wire EDM'ed with +/-.0005" or even closer. Even Machining to that tolerance might be possible.
If you need further help, please let me know.

 

[zdvama]

For the groove I would follow the advice of jjjaos. About the tongue you may permit tolerancing up to 0/-0.001" because easier manufafacturing and measuring. In this way you will accept the advice of gearguru, because the ISO system of fits offers fit like this.
Good luck!

 

[m4kert]

I agree with the advice of jjjaos, but with one exception. You need to consider the length of your parts. If your mill bed can handle a 3 foot part, great, but if more than one set-up is required, I would add a little more to the "fit". Talk to your machinist. He/she will give you a better idea of what the mill can do. Some mills aren't refurbished properly.

 

[Woody1]

All of the information given here is good but if you want the best possible fit, then you need to make a change in the design and add an adjustable gib to the groove. This will allow a true sliding fit with no side to side play.
Otherwise follow GD&T guidelines for fits and dimensional tolerance stack-up. Woody Ebersold
Consulting Engineer
"AN EXPERT IS ALWAYS SOMEONE FROM OUT OF TOWN"

 

[John2002]

Hello,

I just wanted to thank everyone for their replies to this post. I have received some interesting feedback, & I like hearing all the different points of view. Someone had pointed out that the length of the parts is a factor. I forgot to mention the length (1.375&quot in my original post.

At the website

http://www.engineersedge.com

under the DFM section, it states that bilateral tolerances should be used with CNC due to "cutter compensation". However, I am not sure if this would apply to my situation. I have pasted the link below if anyone wants to take a look.

Thanks again.

John

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

 

[minasian]

Hi . I advice you to use the Iso tolorancing tables to find out it , but I should tell you that the correct answer for each case is found by try and error .if you have the chance of it .because many many items infect the tolorancing ,such as heat transfer ,vibration, material,machining quality , so you should consider all of this .Although there are many standardised tables for different items , for exmple bearings,pullys,gears,o-rings and also some examples for different clearanses but if you case is a uniqe one you should find it out yourself by trying different standard tolorances from ISO tables considering other parameters like manufacturing , cost and ...

Good luck
Alan Minasian