PDA

View Full Version : Dovetails



QSIMDO
04-11-2009, 02:44 PM
When cutting an internal dovetail, should the cutter be sized to only cut one wall of the slot at a time then progress in size?
Or can the cutter do both sides at once?

websterz
04-11-2009, 02:51 PM
Remove the bulk of the material with an endmill, leaving a square channel just narrower then the width of the small side of the dovetail. Make all your dovetail cuts against the fixed jaw...ie make a cut, turn the part, make second cut, then measure. Repeat as necessary. This way you are moving the Y axis in only one direction, easier to manage backlash that way. Take small cuts with the dovetail cutter, it will last much longer that way. I made my own inserted 60* cutter and have probably cut 50 feet of dovetail in steel and 6061 wthout indexing the insers, still cuts like new.

John Stevenson
04-11-2009, 04:33 PM
No, don't turn the part, that way can lead to tapered cuts.
Cut the fixed side in one direction, the direction that's not climb cutting, then cut the other face in the opposite direction.

This way you get to cut two parallel faces.

.

uncle pete
04-11-2009, 06:59 PM
John, A exellent point and one I've never considered but makes it totally logical when you think about it. Thanks.

Pete

websterz
04-11-2009, 07:53 PM
No, don't turn the part, that way can lead to tapered cuts.
Cut the fixed side in one direction, the direction that's not climb cutting, then cut the other face in the opposite direction.

This way you get to cut two parallel faces.

.

Just passing along the way I was taught...never had problems with it.

oldtiffie
04-11-2009, 09:55 PM
Why use a vise at all if it is avoidable? A vise can have errors of its own as regards "up-lift" and "out of parallel" but sides of the dove-tails - done as John S advises - will be parallel. If "vise problems" are an issue the dove-tail may not be parallel to the surface that should be resting on the vice base or parallel strips - which is another problem.

I avoid using a vise if possible as I prefer to clamp directly to the mill table or next on parallel strips on the table.

I would certainly get rid of as much material as I could before using a dove-tail cutter and then use conventional milling one side at a time to remove the bulk of the rest of the material. I would finish off with a very sharp dove-tail cutter with my table ("X" or "Y") clamps partly on and finish off by climb milling (only a "thou" or two).

Dove-tail cutters are fine in/on brass, aluminium and cast iron but get more problematical when used on even mild steels.

I prefer the much more expensive "spiral-toothed" cutters to the common "straight-toothed" cutters as the former cut much better than the latter.

Given a choice, I'd use a shaper or a slotter for dove-tails as they are pretty made for it. Next, I'd rough out on a mill and then finish off on a surface or tool & cutter grinder.

Dove-tails can be done very well with a fly-cutter and with either the milling head tilted to suit or alternatively with the milling head left vertical and the job on a tilting table as that fly-cut surface beats a dove-tail cutter and can approach a "spiral-ground" finish - but the set-ups can be difficult.

But as is all too often the case, I/we don't have a choice and have to make the best of what is available at the time.

QSIMDO
04-11-2009, 10:29 PM
The situation is this; I've a channel .5" deep by .625" wide and only a .75" dovetail cutter.
Just from what I can see the cutter is too shallow from the shank to the bottom to make a full depth dovetail and too narrow to introduce the cutter correctly without taking what looks like too much of a bite.
Is there some width/ depth/cutter size formula I'm unaware of?

Paul Alciatore
04-12-2009, 02:02 AM
When cutting an internal dovetail, should the cutter be sized to only cut one wall of the slot at a time then progress in size?
Or can the cutter do both sides at once?

As for cutting both sides at once, it probably has been done. Like cutting a Tee slot. However, it would be better to cut one at a time. This may not be possible if the dovetail is too deep. A well designed dovetail allows for the width of a standard cutter.

Do cut the center out as wide as possible with a standard end mill. It is OK to go a small amount below the bottom of the dovetail with this cutter as this center area is not needed for proper operation. If the resulting slot is too narrow to allow the dovetail cutter to cut on one side only, you may consider other means of roughing things out. A saw blade at an angle might help. Also a small Tee slot cutter could help rough things out.

I have to agree with John S. You really want to cut both sides with one setup. This will help guarantee parallel sides. And avoid climb cuts.

You can use two pieces of drill rod to measure the width. They should be sized to allow them to fit inside the dovetail with space between them for the caliper's inside jaws. But the space between them should be less than the width of the dovetail's opening. A bit of math is needed. Or use a CAD program and draw it with circles to indicate the drill rod in contact with the sides and bottom and pick the distance between the rods from the drawing. I did it that way and made matching male and female dovetails on my first try. They fit like a glove with no gibs for adjustment.

danlb
04-12-2009, 02:37 AM
In a pinch, you can tilt the piece and use a small end mill to rough out the shape of the dovetail. In fact, you can even make a usable dovetail with just an end mill. It will have extra material removed at the bottom of the dovetail, but that does not keep it from working.

The parting blade holder just to the left of center in the attached picture was one of my earliest dovetail attempts. You can see that the 1/4 inch endmill cut into the body of the holder. It does work.

Please ignore the amateurish work. I took that picture to illustrate what could be done with a micro-mill. I'm doing much better now. :)

Dovetail cutters come in many sizes. I picked up a box of three (large, medium and small) on sale from Enco fairly cheap... less than $20.

http://home.earthlink.net/~dbsweb/pieces1.jpg

Dan

oldtiffie
04-12-2009, 06:34 AM
Dan's solution is the best so far as it will work without a dove-tail cutter, but I'd suggest tilting the mill-head to suit and if on a machine where the milling head has a "nodding" (forward-back) feature, mill in one position on the table and cut in the "X' plane, but if you only have a "tilt" (left-right) mill on the "Y" plane.

The dove-tail maths are here:
http://www.homemetalshopclub.org/news/dec02/dec02.html

Marv Klotz has an excellent (DOS-based) utility at:
http://www.myvirtualnetwork.com/mklotz/files/dovetail.zip

Marv's file note (at dovetail.txt within the archive/zip file) reads:

One way to measure a dovetail is to put cylindrical pins into the angles of the dovetail and measure across the pins. Knowing the dovetail angle and the diameter of the pins, it is then possible to derive the measurements across the top and bottom of the dovetail.

This program implements the calculations for this operation.

Any type of units may be used for the inputs so long as the user is consistent and doesn't mix units.

Output units will be the same as the input units used.

So, all the math will be done for you.

.RC.
04-15-2009, 03:23 AM
Given a choice, I'd use a shaper or a slotter for dove-tails as they are pretty made for it. Next, I'd rough out on a mill and then finish off on a surface or tool & cutter grinder.



Just curious why??? I would have thought that using a shaper/slotter would be slightly inferior to a mill with a dovetail cutter as on the shaper/slotter you have to set the angle correct for each side.. Where a dovetail cutter in a milling machine you just zip up one side and down the other, guaranteed to be the correct angle (so long as the dovetail cutter is correct) and parallel to one another..

Then if you make the mating parts with the same cutter they should fit correctly, with only minor fitting needed..

(I just bought a "presto" dovetail cutter off ebay so I have to say the above to justify the expense..Although it was quite cheap for a brand new cobalt HSS cutter)

oldtiffie
04-15-2009, 03:48 AM
Ringer,

dove-tail cutters (with straight teeth) are inclined to "chatter" and the narrow "neck" doesn't help much either - but they can and do do the job - no question.

All too often the collet or its holder is inclined to be too close to the clamps with a dove-tail cutter on a mill.

I prefer the "spiral-shaped" teeth to the straight teeth.

Dove-tail cutters really require a good real or pseudo tool and cutter grinder to get them sharp.

Setting the angle on a shaper/slotter is not a problem. I can set any angle I like plus a shaper/slotter, with a correctly sharpened tool and a good set-up, gives an excellent surface finish.

To get a feel or an idea of this, cut a straight edge on a piece of aluminium first with a straight tooth TC router cutter and then with a spiral milling cutter of the same size. The straight toothed cutter is inclined to "hammer" under load and leave a slightly "corrugated" finish where-as the spiral cutter will get right into it and will leave a much finer/better finish. Its not unlike the difference between HSS straight and helical-toothed side and face cutters on a horizontal mill - or even the difference between a straight toothed and spiral-toothed slab milling cutter on a horizontal mill.