PDA

View Full Version : How to dimension Dovetails on a drawing?



sconisbee
01-08-2010, 04:03 PM
Whats the best easiest, least error prone way of dimensioning small dovetails
on a cad drawing, preferably ISO compliant?

I.E. How would you dimension this dovetail?

http://i59.photobucket.com/albums/g290/synoguy/dovetail.jpg

Thanks

Simon

gda
01-08-2010, 04:12 PM
Expect this thread to go long with different opinions - but to me how to dimension it depends on how critical it has to be, and how good your reference surfaces need to be.

The two simplest options are:

1) dim to theoretical intersection points for width
2) draw in 2 rolls tucked in the dovetails and dimension the width between the rolls. Lots of trig with this one.

If I was doing it at work I would probably be using GD&T and dim to the centerline of the dovetail.

Tony
01-08-2010, 04:21 PM
Dovetails are tricky and you'll probably get a lot of different suggestions.
If you look in GD&T I think there is a "profile" standard.

You don't want to dimension to any sharp corners, inside or out.

Typically, I think these things are measured over gage pins or balls..
you could show those in your cad and dimension center to center. The
"circles" (gage pins) would set your start and end position of the dovetail
(how long it is). And its position, of course.

Just by looking, it doesn't seem that your dovetail is symmetrical to the part,
but if it were, you could take advantage of a horizontal symmetry line and
detail everything away from that. Cleans the drawing up a bit.

Also, depending on whats important on this part, you might want to consider
using one of the holes for a datum instead of the lower corner.

Just my 2c
-Tony

sconisbee
01-08-2010, 04:48 PM
Yeah the dovetail is off center, in this design theres plenty of leeway on the dovetails, they just need to be straight and the right angle and close'ish to dims

I suppose for the mating part the female dovetails are spec'ed the same way just kinda inside out.

Im alright with most drawing just never needed to dim dovetails for anyone other than myself until now.

Your Old Dog
01-08-2010, 05:03 PM
add a gibb to the equasion and it won't be near the problem. You can almost guess it close enough if the gibb is there to eat up the slop ;)

sconisbee
01-08-2010, 05:11 PM
add a gibb to the equasion and it won't be near the problem. You can almost guess it close enough if the gibb is there to eat up the slop ;)

YOD's got it, there will be a gibb used, that's why the dovetail is off center
slightly. I figured it would be easier that way than to expect an outside
source get it spot on first time.

TGTool
01-08-2010, 11:45 PM
I would always dimension over rolls. Inside corners, even if the dovetail mates on the outer flat because that's the most secure way to measure where the surfaces are. I'd calculate from the theoretical sharp corner to design the mating side, but again provide roll dimensions even if I'm allowing clearances on some surfaces.

I had a boss once who showed me how to machine a dovetail for a small slide by measuring with a mic across the sharp corner. :mad: Bullfeathers! He wasn't getting a good measurement because he had no idea what kind of burr was turned up there or whether his mic was crushing the corner. He did it that way because he couldn't do the visualization of the relationships in his head or do the trig to figure out what a roll dimension ought to be. I put up with it for a while then walked.

mechanicalmagic
01-09-2010, 12:11 AM
When applying tight tolerances and dimensions, I always go back and ask the metrology department how they would inspect the part. If I know how to inspect it, then I know how how to dimension it.

So, I went to metrology. And I said to me, how do I measure this dovetail? And I said to me, use gage pins. I usually listen to me, and dimension parts according to things that can be measured easily, with verifiable instruments.

Forrest Addy
01-09-2010, 12:21 AM
Before you dimension the dovetail be sure to identify the face the DT registers aganst. 99 percent of the time it's the double face because of the extra width give rigidity against rotation about the slide's axis. The other one percent the registraton face will be on the single face which is far narrower.

You only have to look at the Aloris type tool holder Vs the piston type to grasp the distinction is real.

In the Aloris type you can dimension between pins or between theoretically sharp inside corners. In the piston type you can only dimension between theoretically sharp external corners.

In the single face DT, it's up to the machinist, the set-up man, or the the lay-out man to identify the intermediate surfaces and references used to indirectly verify the outside dovetail corners of the work piece are in tolerance.

This also applies so the world beyond tool holders. Once in a great while a dovetail is designed to bear on the DT flanks and the single face between them. It's more wobbly but design conditions may force the choice. The dovetail used for DTI's for example.

A critical dimension is missing in the OP sketch: the symmetry/assymetry of the DT to the double face centerline. Here again the dimension can reference a pin centerline or a theoretically sharp corner.

Also. I'm not up on conventions for metric part drawings. In US convention, Integer units are represented with trailing zeros correspondding to the least significant figure in the tolerance: 3.000 +.005/-0.000 for example. I see the "20" dimension has no decimal or trailing zero. Does this denote a stock size face or ref dimension sontrolled by in title block "Unless otherwise noted..." No biggie, just curious about metric part drawing conventions.

Machinist-Guide
01-09-2010, 12:29 AM
Just to put in my 2 cents
Use the 2 point circle tool and snap to the two surfaces of the dove tail
Draw a standard size circle and dim.off the center of the circle.
The machinist would use gage pins to check dim. as they machine.

Paul Alciatore
01-09-2010, 01:09 AM
Just to put in my 2 cents
Use the 2 point circle tool and snap to the two surfaces of the dove tail
Draw a standard size circle and dim.off the center of the circle.
The machinist would use gage pins to check dim. as they machine.

One more tip, perhaps just one cent's worth. If the drawing is just for my shop, I would mike the pins I will uise and use circles at that actual size on the CAD drawing. This picks up a bit more accuracy.

My first attempt at a dovetail was a small aluminum one. About 3/8" high and 3/4" wide. I drew the female about 0.001" wider than the male and used circles the size of the drill rod I had for pins. It went together like silk.

whitis
01-09-2010, 02:51 AM
You opened pandora's box on this one. I don't think I have ever seen a well dimensioned dovetail drawing. One that specifies all the critical dimensions and allows some slop where it doesn't matter. I.E. one that was neither over or under specified. More than a century after the invention of interchangeable parts, dovetails often fail to be interchangeable.

If you dimension over pins and they need to use a different pin diameter, it makes a mess of things. What if they use a coordinate measuring machine? What if they use two or more different size pins for measuring which gives a better check than one size? What if they use dovetail gages or dovetail calipers? With dimensioning to a pin, you are making the measurement at one arbitrary height have particular importance that it does not in fact have in the actual operation of the part and which may interact with other tolerances. And which surface is the pin referenced to and is it the right one? If figure 8 and 9 are for mating dovetails, you are measuring against an uncontrolled or irrelevant surface on either the male of the female, depending on which flats are supposed to mate (see figure 3 to understand what the preceeding phrase means):
http://www.neme-s.org/Model_Engineer_Files/Gauging%20Dovetail%20Slides.pdf
At least one of the pin measurements needs to be made against a surface plate because the pins have to use the imaginary line between flats as a reference surface:
http://books.google.com/books?id=4Q8LAAAAIAAJ&pg=PA366

Draw the ideal profile and dimension that. Tolerances are from the theoretical profile. True position.

Show a radius on the edge of the dovetail and have dashed lines meeting at the theoretical intersection point and dimension to that point. Or draw solid and put an arrow with an radius or chamfer dimension on the point.

Here is one typical example from American machinist's handbook.
http://books.google.com/books?id=4Q8LAAAAIAAJ&pg=PA365

Consider whether you should put stress relief holes/groves at the base of the dovetails. Otherwise, you have stress risers. These also allow you to get a reference edge in there and allow clearance for chips. Can be a pain to make, though. You can also have radius's on the inside corners with ample clearances and get some of the same benefits.

What are the reference surfaces for your dovetail? The two angles, obviously. But what of the flats? Assuming the male dovetail points up, does your female dovetail ride on the flats on the top of the male dovetail or does it ride on the flat surfaces either side of the male dovetail?
See Figure 3: http://www.neme-s.org/Model_Engineer_Files/Gauging%20Dovetail%20Slides.pdf
Once you have dimensioned your dovetail, pretend you are Murphy. How can you deviously make a part that meets those dimensions but fails to work properly such that it makes a lousy slide or the parts are not interchangeable?



Some dimensions to consider:
- The angle of the dovetail in degrees or rise/run. Critical.
- flatness of the 4 reference surfaces on each half of the dovetail
- surface finish of the reference surfaces
- parallelism of the reference surfaces to each other and other features of the part.
- radius/camfer on the corners of the dovetail. Your outside corners better fit inside your inside corners.
- Width of narrow side of dovetail (both male and female)
- width of wide side of dovetail (both male and female)
- height of dovetail (male and female)
- dimensions of the reference surfaces - how wide are the reference surfaces over which the dimensions must hold?
- stress relief holes or grooves in corners of dovetail
- undercut between reference surfaces on female dovetail if you ride on the "top" of the male dovetail.
- gib dimensions
- oil grooves?
- matching between multiple slides in the same assembly, if applicable
- tolerances on above dimensions
- true position error?
- are you dimensioning against uncontrolled surfaces? For example, is your dovetail angle measured reference surface to reference surface or is it measured reference surface to irrelevant surface? What happens to your dovetail angle if the irrelevant surface happens to be tilted at 1 degree?

Design so the minimum number of dimensions are critical, or pay through the nose for precision where you don't need it or shouldn't need it.

In addition, you may need allowances for rescraping. The original spec should guarantee that there is sufficient material for rescraping, but less material will be present after rescraping. So, you need a design that allows this and two sets of tolerances. The original tolerance has a minimum material condition that allows material to be removed later. But if the part barely meets the minimum material condition, then the rescraped part cannot. Also, wear tolerances beyond which the part needs to be refurbished.

sconisbee
01-09-2010, 02:57 AM
Before you dimension the dovetail be sure to identify the face the DT registers aganst. 99 percent of the time it's the double face because of the extra width give rigidity against rotation about the slide's axis.


Also. I'm not up on conventions for metric part drawings. In US convention, Integer units are represented with trailing zeros correspondding to the least significant figure in the tolerance: 3.000 +.005/-0.000 for example. I see the "20" dimension has no decimal or trailing zero. Does this denote a stock size face or ref dimension sontrolled by in title block "Unless otherwise noted..." No biggie, just curious about metric part drawing conventions.


Thanks Forrest, Please excuse me being stupid (its 8am and i havn't woken up fully yet it was a late night) which face is the double face? The face thats actually on the main part? or the face thats on the outside of the DT, as im assuming by flanks you mean the angled parts of the DT?.

As for dimensioning metric drawings, yes as far as i know and all the drawings i've ever dealt with have been dimensioned in the way you described, this one will be also once i have nailed down the dovetails.


Everyone else, thankyou for the advise, keep it coming, ill tinker with the drawing and post back in a bit, it seems like measuring over rolls is the best way to dim it, makes sense when i think about it.

oldtiffie
01-09-2010, 04:04 AM
Most of the required dimensions are here:

http://i200.photobucket.com/albums/aa294/oldtiffie/Sketches/Dove-tail_dims1.jpg

Circlip
01-09-2010, 04:30 AM
Look in any of the Model Engineer mags with articals written by the old "Masters" and you will find the two roller method is used for checking both internal and external Dovetail forms. Given that you've allowed for a gib strip, the tolerances are not too important except if you want to sell the finished item on here, as you'd be competeing with the Chinese tooling companies. Tiffe has noted Knocking the corners off the female part, you need to do the same on the sharp bits of the male part.

Used to get a bo**ocking for doing the "Equi-centred" dimension symbols cos it's not STRICTLY correct, but it does show your intentions as to what fits where.

Regards Ian.

spope14
01-09-2010, 04:05 PM
Checking a dovetail for linear dimension is done over gauge pins, the inspectors or QC department of whatever company determine the gauge pin size and calculations (as shown above). I checked my old textbook Technical Drawing (Giesecke) and it shows the standard practice of dimensioning dovetails using the note "TO SHARP CORNER", which is how you draw them anyway. Female dovetails are dimensioned to the opening, or smallest part. male are dimensioned to the tips of the widest part, or top of the male. Angles are also dimesnioned as is depth. A couple of drawings also listed "to gauge", which would be the gauge pins, and also noted the flats or inner radius dimensions that dovetails have (but do not affect the sharp corner dimensioning).

J Tiers
01-09-2010, 04:11 PM
The gage pin method is tantamount to measuring the "half height", or what might be considered the "pitch circle" as if it were an infinitely large gear (in reverse).

it should probably be the ONLY method used, but you naturally need to specify the pin size. That will allow calculating the size for any other pin.

brian Rupnow
01-09-2010, 04:44 PM
When dimensioning dovetails, you require two sets of dimensions. The first set are "Reference" dimensions, and are to the theoretical "sharp points" and must be marked (REF) so that it is clear they are for reference only, not to be machined to. The second set of dimensions must be to something which can actually be measured by the machinist making the part----Consequently a dimension either "out to out" or "center to center" of gauge pins (dowels) of a known diameter.---Brian

J Tiers
01-09-2010, 04:48 PM
Why do you need the others?

The angle and the pin measurement give it all, except for overall height etc..... and finish of the sharp corners, in terms of relief etc.

spope14
01-09-2010, 05:19 PM
J, in theory, you are correct, and man that would make the job easy. This said, I bring up this example. In a shop I worked in last year, they had "process checks" for a dovetail based over a specific set of pins. A large production job (seven figures of parts, so inspection had to be very standardized to production, not to "trigging out" all the time, someone already did this). The dimensioning was done to the top opening of a female dovetail on the actual finish print.

To make a long story short, over the course of a week, the specific pins were lost in coolant tanks, the floor, or wherever pins go to take vacation. Using the specific dimensions, triging the problem out, production went back on line in minutes with pins .003 larger in size. If a dovetail is listed to size "over pins", then you must have the specific set of pins. When you change pin sizes, you have two factors that also change, the tangent points from the bottom and the angle of the dovetail to the center of the pin.

In my own shop, I am sopmewhat limited in duplicate pins, so when I teach dovetails, I have to actually teach triging the measuring factors to two different size gauge pins (which really teaches them the process!), though more often than not, I do use dowel pins (though this is not the best practice) to get to "close dimensions".

The bottom line though in this all is that dimensioning of dovetails is a combination of a draftsman training, the company standards, who taught them, or all of the above - be it CAD or pencil.

oldtiffie
01-11-2010, 06:40 AM
There was some discussion on measuring as well as dimensioning dove-tails.

This may assist further:
http://i200.photobucket.com/albums/aa294/oldtiffie/RMIT_book_details/RMIT-P199_1.jpg