×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

DOVETAIL DIMENSIONING
3

DOVETAIL DIMENSIONING

DOVETAIL DIMENSIONING

(OP)
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...

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

(OP)
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...

RE: DOVETAIL DIMENSIONING

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.  

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

(OP)
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...

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

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

Mike Halloran
Pembroke Pines, FL, USA

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

(OP)
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

Quote:

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

Quote:

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...

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

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

RE: DOVETAIL DIMENSIONING

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
   

RE: DOVETAIL DIMENSIONING

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.  

RE: DOVETAIL DIMENSIONING

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.

RE: DOVETAIL DIMENSIONING

(OP)
Well I've pondered over the above, looked at the figures Ron listed and looked at parts of 14.5.

6.6.1.1 caught my eye and seems like "EACH ELEMENT" might apply to exactly this type of situation.  Sadly both examples (6-44 & 6-55) are for cylindrical items but I think it can be made to work.  

Take a look at the attatched sketch and see if you think I've got it right.  I've put C as the secondary datum since only elements perpendicular to C need to be parallel, this is the part I'm least sure about.

Obviously it will need other dimensions/controls but I think this addresses the specific question my colleague asked.

So, what do ya reckon?

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

RE: DOVETAIL DIMENSIONING

KENAT,

  I breezed through the threads so forgive me if this has been answered but; Why the insistence on calling the two angled surfaces parallel? Drawoh brought it up but it was apparently ignored. A surface can only be parallel to one datum plane, not two. See 6.6.3. Only an axis can be parallel to two datum planes. Also, all the points on the surface must be equidistant from the datum plane. All the points on your specified surface are grossly NOT equidistant from neither datum plane D nor C.
  I think you should use composite profile.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

RE: DOVETAIL DIMENSIONING

(OP)
Powerhound, I mentioned in my OP "The term parallel keeps getting used but isn't really correct." I didn't ignore this fact, I'm well aware the surfaces aren't parallel.  On the sketches I put parallel in "" to try and make it clear it wasn't really parallel.  However, it has caused confusion to several so I'll try and learn from my mistake in future posts.

Quote:

6.6.3 (d) a tolerance zone defined by two parallel lines parallel to a datum plane or axis, within which the line element of the surface must lie.  See Fig. 6-45

It was this that I was trying to invoke.  The line elements perpendicular to the end face C, should be parallel to surface D.  However, looking at it again  I'm even less confident that I'm correct.

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

RE: DOVETAIL DIMENSIONING

KENAT,

   There is no such thing as a "line element".  Your face can be perpendicular to datum_C and located in profile from datums_C and_D.  Angle specifications are valid from datum_C and_D, although they are redundant from_C if there is a perpendularity specification.

   May we see the mechanism this is part of?  This would all make much more sense if we understood what it was to do, and what it interfaced with.  I would probably use the top face as datum_A, for example.

                         JHG

RE: DOVETAIL DIMENSIONING

(OP)
Drawoh, there is such a thing as a line element, 6.6.3.1 says so and 6-45 shows an example.  

However, I believe you're correct that for my situation it's not applicable/nonsensical.  I was trying to apply it in a way that I don't think it's really intended to be.

Thanks for all your posts on this subject * for you.

The sketch is much simplified from the actual part, in fact I believe the design may be different from how I'd originially understood it so until I have all the details I don't know how much I can add here (or help him).  For you specific point though, A mounts to a 'bridge' over the top of the tool.  The optics assy has the male portion of the dovetail which then slides into this.

His basic question though was I suppose how to control the variation in width(/orientation?) of the dovetail along it's length.  The actual width had to be controlled to say +-.005 (or equivalent) but he wanted the variation in width to be less.  I'm still not sure I'm expressing myself clearly and my second sketch didn't help much.  

Say the width is nominally  1" with the +-.005 tol.  If one end of the dove tail is 1.005 then he didn't want the width at any other point on the dovetail to be less than say 1.001.   However if the end was .095 then he didn't want the width at any point to be more than say .099.  Does this make any sense?

His idea was to have a note saying that the female dovetail was to be machined in a single step by an inverted V shape cutter as this would be definition keep the width of each dovetail fairly constant to itself.

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

RE: DOVETAIL DIMENSIONING

(OP)
OK, I think I'm starting to get what a coupld of you put, actually read and started to understand 6.5.9 composite profile.

Sorry for being so slow and thanks for your patience.

Though that said, it would allow the dovtail to be located looser with respect to ABC and then the form of the dovetail itsel to be controlled more closely but I'm still not sure it directly addresses his concern.  

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

RE: DOVETAIL DIMENSIONING

A note as you describe could cost you a lot of money.

Making a dovetail "one step to size" is not usually done, even in wood.  Milling cutters, and I think dovetails especially, have problems with tearing material on exit, so it's customary to cut such a groove by entering from both ends.

Making it in one _clamping_ is possible, but still not guaranteed to get you what you want.

As you clearly understand, it's better to specify what you want, than to specify how to get there.

Mike Halloran
Pembroke Pines, FL, USA

RE: DOVETAIL DIMENSIONING

(OP)
Thanks Mike you've helped confirm my concerns about trying to specify the machining step (which of course contravenes the standard anyway...)

He claimed he'd seen this from an optics supplier or something but it still doesn't sound like a great plan to me.

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

RE: DOVETAIL DIMENSIONING

KENAT,
  I think what you are trying to achieve is on page 168, FIG. 6-16. I think this is a better representation of the concept in 6.6.3(d) than FIG. 6-35. The fact that the linear elements are 2 dimensional allows then to be used with 2 datums, like an axis. The problem with your sketch is that the callout is in the wrong view.
  Honestly I still think composite profile is your best solution but if what I've mentioned is what you were after, I can now see what you were trying to say.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

RE: DOVETAIL DIMENSIONING

(OP)
Powerhound, thanks, I think that image is kind of showing what I was trying to achieve.  I'll have to have a think about how exactly to show it clearly/unambiguously but I think that's it.

Thanks, star for you.

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources