DOVETAIL DIMENSIONING 3

[KENAT]

I have a colleague that is designing both the male & female halves of a dovetail joint. The dovetail is used for a detachable optical assembly and variations there on have been used with adequate performance for some time at my employer. However since most of those were introduced the company has become more aware of tolerance/repeatability issues and is now using GD&T (ASME 14.5M-1994).

He has asked me how I would keep the angled edges in the same alignment, ie effectively keep the width of the dovetail the same to a fairly tight tolerance. The term parallel keeps getting used but isn't really correct.

My initial suggestion was just to control the surfaces with surface profile however he doesn't seem convinced by this. He is very concerned about keeping them aligned but doesn't seem as concerned by other factors. My other suggestion was to call out a fairly tight perpendicular tolerance to the end face but while this would help keep the edges aligned it isn't really necessary for the dovetail to be highly perpendicular to the end face.

Now I'm not convinced he's correct as once installed a screw pushes in from one side pushing the dovetail to the other, so I don't see why they need to be tightly controlled but he's convinced.

He wants to call out the machining process, saying they are to be machined in a single step but obviously this doesn't fit well with standard drawing conventions, I'd rather detail the end requirement not how to achieve it.

Any ideas appreciated, simplified sketch attatched to give some idea of the female.

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

 

[vc66]

Once in place, the male and female are "locked" together, via a screw? If that's the case, I don't really see why the sides need to be so tightly controlled.

If he really wants them to be controlled very tightly, then I would suggest a surface profile tolerance, as you first suggested.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

 

[drawoh]

KENAT,

Faces cannot be kept parallel because they are not parallel. They look closer to perpendicular to me.

Actually, I cannot see a dimensioning scheme other than a GD&T profile tolerance. Your maximum and minimum widths are to theoretical sharp corners which will be round on the actual part. You are interested in the position and form of the surfaces. The radii can be fairly sloppy.

I would call up a composite tolerance consisting of profile and angle. The profile tolerance would reflect the positioning requirements of your dovetail, and the angle tolerance would be accurate enough to ensure proper mating.

JHG

 

[KENAT]

VC66, I agree and I'll have the discussion with him again but he's more senior than I and just doesn't seem to get it. Doesn't help that my arch nemesis (no I don't treat him like that etc) when it comes to quality drawings, applying GD&T etc reports to him and has I'm sure filled his head with all kinds of ideas.

"Faces cannot be kept parallel because they are not parallel" my point exactly.

Drawoh, if you don't mind me being dumb, could you expound on what you say about angle tolerance. I take it you mean the angle of the 2 V survaces to each other? With your scheme the angle tolerance will be tighter than would be expected from the surface profile alone?

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

 

[CheckerRon]

KENAT: I too wonder how drawoh would apply both profile and angularity to these parts.
1. If we talking about the dovetail mount on the removable optical assembly, I would "profile of the surface" dimension that dovetail similar to Figure 6-23 of Y14.5, except linear, not diametral, with the FCF on both angular surfaces. The mounting surface being datum A, the large end of the dovetail width being a centering datum B, and the end that serves as a stop being datum C.
2. On the left and right mating dovetail parts (seperate pieces I think), control them too by profile of the surface with a Basic angle relative to a three plane datum system on each dovetail half, or use an angular tolerance IAW Fig. 6-27. The result is the same.

 

[drawoh]

KENAT,

You apply a profile tolerance of 0.5mm and an angular tolerance of 0.1mm. Both tolerances specify the acceptable variation.

The profile on its own allows an angular error of up to 0.5mm, assuming you had absolutely no error anywhere else. The additional angular tolerance controls the angle down to 0.1mm, but the angled form is allowed to be as much as 0.25mm off the nominal position.

I am assuming your angle is very much more important than the location of the profile. Figure 6-23 controls an entire form with a precision you probably do not need.

JHG

 

[KENAT]

Thanks, I'll take a look at those figures in the standard when I'm back at work.

I realized I may not have stated my question clearly so I've added another tiff to try and make it clearer. It trys the show the situation he's concerned with avoiding.

Ron, it's sort of the application you're talking about but on a new tool on the other side of the business, the female is I believe a single part not 2 as on the ones we dealt with before.

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

 

[drawoh]

KENAT,

I assume the top and bottom edges are to be parallel.

The parallel specification usually applies to surfaces, which in your case still are not parallel. Your edges are hard to describe and inspect given that they will be manufactured as radii. I suppose you could apply parallel specifications to the edges, but the inspection would be difficult. You really are interested in the surfaces.

If the angle is more critical than the location and separation of the two surfaces, my composite tolerance, above, should still be a good solution. It is possible you only need the angle specification on one side.

JHG

 

[btrueblood]

Alternatively, specify the angle as a basic dimension, and use profile tolerance only?

 

[MikeHalloran]

The traditional way to measure dovetails is over or between gage balls or gage bars.



Mike Halloran
Pembroke Pines, FL, USA

 

[CatMann]

Dear All,

Nice to see your discussion...I have given a hit here...
Pl. correct me if I'm wrong..

CatMann

 

[btrueblood]

The sharp corners bug me, but then, I don't have to machine it.

 

[KENAT]

I'm caught up on something else but will get back to this.

In response to some of the comments though...

In the OP I said

simplified sketch attatched to give some idea of the female

The 2 sketches I attached are not excerpts from the drawing, just very simple images to try and help explain my point. As such sharp edges are shown for simplicity, not because the real part will be like that.

In the OP I said

The term parallel keeps getting used but isn't really correct.

so yes I am aware the 2 angled surfaces aren't parallel.

Catmann, thanks for the sketch. I think there may be a couple of items in it that aren't quite correct but don't have time to look more closely right now.

Thanks to all for your time, anyone who has anything to add especially after looking at my second attatchment please feel free/I'll appreciate it.

Ken

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

 

[ctopher]

Have you looked at possibly using symmetry?

http://www.tec-ease.com/tips/september-97.htm

Chris
SolidWorks/PDMWorks 08 1.1
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[vigildesign]

See MIL-STD-1913 for a type of dovetail. Very common.

 

[KENAT]

http://en.wikipedia.org/wiki/Image:M1913A_Rail_CrossSection.gif

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

 

[MikeHalloran]

That's what the gage bars are for.

A gage bar is two gage balls separated by a spacer of fixed length, such that the distance between the ball centers is known accurately. For large ways, it's customary to make them 12" c-c, which simplifies some of the math if you have to do it by hand.

To use them, just nest two gage bars into the way opposite each other, and use gage blocks to measure the distance between the corresponding balls. The 'taper' resulting is usually reported as inches per foot, or mm per dm, or whatever you like.

I have no idea how to do it on a CMM. I have no idea what to do with a CMM.



Mike Halloran
Pembroke Pines, FL, USA

 

[drawoh]

CatMann,

Your figure shows the precise error I was warning KENAT about. Your inside width is shown as XX+0.5/-0. When I take my vernier calipers and measure that, I will get the distance between the quadrants of the radii that occur when the machinist cleans up the sharp edges. The cleaned up edges will be poorly formed, inaccurate radii, probably applied with files and dental tools. This is not a good way to locate the surfaces.

The really critical measurement would be over the gauge balls as suggested by MikeHalloran.

The dimensions to and across the sharp edges must be basic. Your profile tolerance provides all the controls necessary over the feature. You should have notes somewhere on the drawing specifying maximum outside and inside radii.

Your profile tolerance is very accurate. Perhaps this is needed. Perhaps only the angle is very critical. Perhaps only one side of the dovetail requires accuracy. The composite GD&T frame I suggested above allows you to control the stuff that is really critical, and open up everything else.

JHG

 

[CheckerRon]

CATMAN: drawoh brings out good points on your sketch, moreover, Datum A is there for a reason. Why are you not dimensioning to it, rather than the opposing face? The opposing face also needs to be parallel to datum A.

KENAT: Regarding the taper in the plan view of your new sketch, consider the Fig 6-24, (p.275 of Y14.5M-1994)dimensioning method (again, linear, not diametral) whereas the toleranced diameter at 18 BSC is a gaging point for the tapers on both the male and female mating tapers.

 

[gearguru]

I did not read all of the discussion above, I apologize if it was already mentioned: the "width" of the dove tail groove is usually measured using two rollers inserted in the "V" shaped grooves - the distance between the rollers is checked. Some math is needed to get the proper "size between the rollers" and the tolerance.