Centerline/ Symmetry

[iv2jm]

Hey Guys,

I came across an interesting issue. Angles that appear 90 degrees are assumed right angles unless otherwise marked- are centerlines assumed to designate symmetry across a a feature with flat sides? IE, a keyway or hex pattern for wrench.

I have a shaft with a keyway at 22.5 degrees below horizontal. I drew a centerline through the center of the shaft and gave the angular dimension. here is the tricky part... The keyway is .375 +.002/-.000. Is that assumed to be cetnered and symmetric on the centerline, or should i include the half dimension; centerline to one side?

If i dimension to one side for location, the value is .1875 which is not defined in my title block and is also not practical it machine or inspect. if i let it round to the .188 to meet my tolerance block then the .005" is more than double the keyway tolerance!

some suggestions would be helpful. Im trying to keep it simple and not GD&T the whole part. is it possible?

Thanks

 

[fcsuper]

No. Using centerlines is also considered to be a non-preferred method to identify the location of features.

A couple of points:

1.You can use .1875 as the dimension if you wish while still keeping the standard tolerance, it simply means you will have a dimesion like this: .1875 +/-.0050.

2.Machining can be done to .0005 without much of an issue. It may cost a bit more, but it is still practical (depending on methods employed by the vendor, of course). If you don't need to do it though, then don't.

You have to determine what is the most significant part specification on the keyway and then base your dimensioning scheme on that.

Could you upload a picture of what you mean so we can have a visual?


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

 

[fcsuper]

Let me correct myself, using centerlines to presume a tolerance without a dimension is not preferred and isn't supported by the standard.

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

 

[KENAT]

As fcsuper more or less says, although it's common to see centerlines implying symmetry this is not supported by ASME Y14.5M-1994 as I understand it.

You say you don't want to use GD&T but I think what you are trying to do would suit either position or surface profile tolerance.

As to 4 place decimals not being in your tolerance block, assuming you work to ASME Y14.5 or similar then you can add a 'non standard' tolerance to an individual dimension, you don't have to rely on the block tolerance. In fact over reliance on block tolerance can be a bad thing as it may mean you aren't really working out the tolerance based on function.

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

 

[drawoh]

iv2jm,

If you show an object symmetric about a centreline, with dimensions to the centreline, I would assume symmetric geometry. The half width dimension is a waste of time, since the centreline is an imaginary element we cannot measure to or from.

My experience of GD&T is that it makes my drawings simpler and clearer. You apply tolerances to the width and length of your slot, then apply a location tolerance to its position. Profile tolerances are potentially even simpler, but would not allow as accurate a slot. Mostly, this depends on your application.

I would not apply an angular dimension from the centreline of a shaft. I would select a feature, and apply the angluar dimension from that. I would not leave this to the imaginations of your machinists and inspectors.

What does define your centreline? Is it a face and a diameter? Is it two diameters? Do you have a long, cylindrical feature? GD&T datums mean that you control this definition.

JHG

 

[CheckerRon]

Good answers, especially drawoh, who must be either Canadian or British (centre). My first thought also was 22.5° from what real, measurable feature? The shaft diameter is (I would assume)the centering datum for your keyslot and the keyslot should be positioned and toleranced to it. The centerline assumes the center of the shaft, but what if it is off center? What tolerance says that it is out-of-print?

 

[iv2jm]

Thanks for all your tips. Ive attached the pics- one is the keyslot, and the other is a hex on the end of a shaft. The hex is dimensioned how its been done in the past- sometimes with the centerline dimension i mentioned before. I agree that this isnt very appropriate, but its also fairly easy to understand what we want. But, like drowah mentioned, my machinist and inspectors can have some pretty wild imaginations. I just want the hex centered and with equal sides/angles (within reasonable tolerance).

As far as dimensioning the most critical factor of my keyslot goes, i want the theoretical centerline of the flats to pass through the center of the bore/shaft. Thats why i showed it.

In this case, since i already have dowel pin holes with GD&T features, it wouldnt be a big deal to use another datum. we do have other features (like the hex) that are similar but less critical, where the centerline symmetry would be the only GD&T'd feature. We use a lot of small machine shops due to some very short lead times and there is concern that some of them would ignore or not understand the GD&T if they dont think its necessary. thats a whole other issue!

Thanks again, feel free to tear me apart

 

[KENAT]

Your link didn't seem to show anything.

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

 

[iv2jm]

Eng-tips must not support .jpeg. Or i am not qualified to use the attachment tool... Probably the latter.

This one seems to work.

Thanks

 

[drawoh]

iv2jm,

Your attachment worked this time.

I suggest that you apply a positional tolerance to your slot width, using Datums_A and_B. Use the width of your slot as datum_C. You need a good zero point for your angles, and I think the slot is way better than one of the holes.

If the clocking of your holes matters, add this datum to their specifications.

Alternately, consider what is engaging your slot. Can it move to pick up your accurate slot? If not, a profile tolerance would be a better idea, since it would define the MMC that a key will fit into. Still call the slot up as datum_C. If the slot gets sloppier, you should consider calling up this datum_C at MMC.

I would rotate the part so that the slot is orthogonal. There is no harm locating holes at weird angles.

JHG

 

[desertfox]

Hi iv2jm

I think you should make the angle to the keyway a basic dimension and then use a symmetry tolerance on the slot width.
In addition shouldn't the dimension from the centre of the bore to bottom of the keyway also have a tolerance?
I am talking about the 1.78" dimension.

regards

desertfox

 

[iv2jm]

I just rotated the part so the slot is orthogonal- that should have been the first thing I did.

drawon- I'm not sure how to put a position tolerance on the slot- If I use the width as datum C, does that call my centerline as the datum feature? I can specifically call out the center of the width as my datum, but it seems like I'm back where i started- with an imaginary feature to reference from. Also, if the centerline is a datum, then by definition does it pass through the origin unless otherwise noted?

fox- the angular location isnt as important as the side walls being parallel to the centerline- which must pass thru the center of the bore. so it seems that a basic dimension is unnecessary- but i could be wrong. And the 1.78 is taken care of in the title block.

Thanks again guys. i appreciate the help.

 

[desertfox]

Hi iv2jm

Well seeing as you have now made the slot orthogonal then you can use a symmetry tolerance on the slot width which
positions the sides relative to the centreline.
I assume that none of the holes need to be positioned
relative to the keyway.

regards

desertfox

 

[KENAT]

If I'm understanding you, take a look at figure 4-6 para 4.4.3 of ASME Y14.5M-1994

If you make the width of the slot your datum C then you're essentially making the CL of the slot the datum for 'angular orientation'.

It's not whether a dimension is 'important' that decides whether it's basic, it's whether it's being used to locate a feature that is controlled by position or similar tolerance.

In your case you may want to consider locating the slot with a positional tolerance. Take a look at 4-6, also some of the examples in section 5 if need be.

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

 

[iv2jm]

I don't know how i missed that. I looked through the standards for a while before i posted.

Thanks for all the help.

 

[fcsuper]

Yup, i agree with Kenat. He is prolly the most qualified checker I'll never meet. lol

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

 

[drawoh]

iv2jm,

I think KENAT answered the question you directed at me.

Take a close look at the shaft and key that engage your hole and slot, and make sure you understand were the key is going to be located. This affects your tolerancing scheme.

If you apply a positional tolerance of .01" to your slot, it could be impossible to assemble a rigid, symmetrically located key.

If your shaft and key have some float in them, a rigidly located but possibly off-centre keyway works and could even be a good idea.

A profile tolerance on each side of the keyway will impose a symmetric MMC. Your LMC may have to get sloppy to keep this fabricatable.

Both dimensioning techniques are valid and conform to ASME Y14.5M-1994. Probably, only one of them meets your requirements.

JHG