Announcement

Collapse
No announcement yet.

Dove Tail Question !!!

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Dove Tail Question !!!

    I am starting to put together a retractable tool bit holder kind of like the one Alan Pinkus has put together but my own version. I ordered the dove tail cutters in two sizes just to make sure I have the ones that will do the job ( I hope). My question is, does it really matter how deep or how wide I make the tails? Can you just use any size that does the job with the size material you have? I looked thru the site and found a lot of good info on cutting the tails but didn't find anything on any sizes. I am making my holder with some thinner material and have never cut dove tails before. I held up on making some of the parts well waiting for the cutters because if the dove tails don't come out I may just trash the whole idea. The dove tails seem to be the biggest hertlle in this whole tool for me to make but with any luck it may work out for me. Any ideas on this would be helpful Thanks John

  • #2
    I believe what you are asking is if the major diameter of purchased dovetail milling cutters corresponds to a "standard." If that is the true question of your post, then "no, they do not." There are typical, round figure dimensions which cutting tool manufacturers will use, but these have no relation to any standard width of dovetails. Dovetails can be any width required by the part. The only limiting factor is strength of materials and all the engineering factors which I could tell you nothing about From a machinists' perspective, dovetail depths/widths only matter in that they precisely mate with their other half. There is no "size" to "hit."

    More important is the premise which your question might rest on. I very strongly encourage you NOT to take a full width cut using your dovetail cutters! This sets up a situation where the cutting forces are balanced except at either the entrance or exit of the cut. What happens there... *snap* When cutting dovetails, I would recommend using a smaller dovetail milling cutter than the width of your roughed out trough. Cut one side at a time. Use a conventional cut rather than a climb cut. After cutting one side, do the other with the corresponding feed and cutter rotation (conventional) the same. This lets you fine tune the width to match the other half. Take a small cut on the following side, measure, adjust depth of cut, take another cutting pass, measure, etc. ...until you're right where it fits.

    [EDIT:] I might also add -- the Alan Pinkus retractable tool looks essentially to be the design by George H. Thomas as presented in his book, The Model Engineers Workshop Manual, Ch. 11 - Retracting Toolholder for Screwcutting. Interestingly--in relation to your comments--Graham Meek mentions in Projects For Your Workshop, Vol. 1 that his tool design purposely avoided the dovetail of G.H.T.'s. Thus, Mr. Meek calls his version a "simplified retracting toolholder for screwcutting."
    Having been told once by Neil Hemingway that in his experience most model engineers fought shy of the manufacture of dovetail slideways, I thought that this cylindrical design might appeal to those who wanted a retracting toolholder but were unwilling to do dovetails. Meek, p40
    Last edited by Arthur.Marks; 02-05-2015, 01:45 PM.

    Comment


    • #3
      a wider tail is more precise, a certain amount of play in a wider dovetail will give less deflection as the same amount of play in a narrower dovetail.
      a deeper dovetail will be stronger

      Comment


      • #4
        If you are making a retractable tool holder, then I would assume this dovetail is a horizontal slide for that retraction action. So strength is of paramount importance. I also assume that this dovetail slide will be oriented in a vertical plane; that is one side will be above the other.

        You do not make any mention of the size of this holder but I would recommend a dovetail depth that is at least the size of the tool bits you are going to use. 3/8" deep dove tail for 3/8" tools, etc. Or more. That is my "seat of the pants" suggestion, no calculations were made.

        I have cut a couple of dovetails and will offer some additional comments. First, you should "hog out" as much material as you can with a square cutting milling cutter. Many female dovetails will show a shallow depression down the center from such cutting action. You can also remove a lot of material from a male dovetail with such a cutter. This lightens the cutting load on the more fragile dovetail cutter. This "hog cut" on the female dovetail should be wide enough so you can start the dovetail cutter with contact on one side only. Do cut each side separately, as others have suggested.

        Getting the size/fit between the male and female dovetails correct is another problem. If you plan to use the mating part to get the fit correct on the other one, you can easily overshoot the mark and wind up with excessive play. If you use a gib, this problem is minimized, but many dovetails need a precision fit. Even with gibs a precision fit can be highly desirable. One way, the way I used, to get this is to measure the dovetail with precision, round pins. I used a CAD drawing with the male and female parts drawn to precise scale, with an allowance for proper fit of 0.001". That is, the male part was drawn 0.001" wider than the female part. Then I drew circles inside and outside of the dovetails with a measured diameter of some ground stock I had. Finally, I added dimensions for the space between these circles on the female dovetail and for the outside to outside dimension on the male part. This gave me some exact figures to shoot for in the mill. The pins that were cut from that ground stock were inserted in the partially cut dovetails and measurements were easily made with standard micrometers and calipers. I transferred the inside measure from my dial calipers to a micrometer for better accuracy. I was able to hit a good fit on the first try using this technique.

        Make a decision on which of the non angled surfaces of the dovetail will actually be in contact. For best fit, you should use only two such surfaces: most dovetails have four possible ones, the two outer edges and two inner edges. On one of the parts, male of female, these edges are also cut by the dovetail cutter while it is cutting the angles. On the other part it is the original, outside surface of the stock. For maximum strength and stability it is best to use the two outer surfaces. Do not try to have all four of these surfaces in contact. Leave some clearance on the other two. And before cutting the dovetails, do finish the outer surface of the part where that surface will be utilized as part of the fit. But keep in mind if you use my round pin method of measuring the dovetail, then all of these surfaces will be involved in that measurement and all four of them must be machined to size as shown on the CAD drawing used to determine the dimensions.
        Paul A.

        Make it fit.
        You can't win and there is a penalty for trying!

        Comment


        • #5
          Thanks ALL for the replays and I guess I got this kinda figured out. I would like to see how Mr.Meek made his tool but couldn't find anything on line about it. The biggest thing I was worried about was how deep the dove tails really had to be and by the replies I will make them as deep as possible for the material I am using. I am using two pieces that are both 1/2 in thick so I think I can work out a good depth so the dove tails will still be strong to hold the tool holder tight.

          Comment

          Working...
          X