Announcement

Collapse
No announcement yet.

cutting very deep keyway

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

  • cutting very deep keyway

    I have a print for a part that shows something like a semicircular Woodruff key slot. The with is .105" and radius is .940", but the depth is such that the shank on the cutter could be no more than .120".

    The part was produced as a casting, but the prototypes were done on an ordinary Bridgeport-style mill. There's a small chance that this particular cut might have been done via EDM.

    The print calls for a flat bottom and square corners.

    The best I've thought up so far is to make a fixture to hold the part to the rotary table, turned up on its side, and rotate the part under an end mill, lowering the end mill for every pass. The floor of the groove would be curved, though. Not as much as a ball mill, and it would function properly, but it still wouldn't be per print.

    Here's the relevant part of the blueprint:
    http://i1267.photobucket.com/albums/...X302/bolt3.jpg

    With the depth of cut at .180", that's .060 max radius for the cutter shank, .120" diameter.

    Anyone have any suggestions?

  • #2
    Whiskey Tango Foxtrot.

    Man, someone needs a beating for drawing up something that gastly.

    I don't have any woodruff standards handy but that seems wrong for a key slot.

    First thing, is it something you are making for yourself or a job?

    If it's for yourself analyze what the slot does and assess if it needs to be that deep or if a radiused bottom is ok.

    If it really needs to be flat, cut it to depth with the method you proposed and grind the shank of a woodruff cutter to finish it off.

    I'd make sure the woodruff cutter is narrower than the slot to minimize loading. In other words, do one side and move it over to finish the bottom.

    The title suggests gun part, what's the hole near the bottom for?

    Chris

    Comment


    • #3
      It's the bolt head for an antique gun. The keyslot is for the extractor. The blind horizontal hole on the bottom is for the ejection plunger.

      I would do things differently if it was my design. Right now I'm trying to replicate the original as closely as possible.

      Comment


      • #4
        A standard #304 cutter will do that very well if you grind the neck diameter down from .160 dia to .110. I think I have one already ground at work. The diameter of most keyseat cutters is smaller than the nominal. They say it is a 1/2" cutter but it is usually about .485 - .490. If not then just regrind the cutter to the right size.

        Comment


        • #5
          Yes, but that's a .500" diameter cutter. A .110" shank seems awfully small for a .940" cutter!

          Comment


          • #6
            Originally posted by TRX
            Yes, but that's a .500" diameter cutter. A .110" shank seems awfully small for a .940" cutter!
            He wrote .940 but look at the drawing. It says .240R,+.005/-.000. That is .480 to .490 diameter. Methinks it was a typo Cap'n!

            Comment


            • #7
              .240 radius... .480 diameter. Arrrgh. I'm going to kick some dirt over that and pretend it didn't happen.

              Is a .110-.120 shank really enough to do the job? Should I make a clean cut into the metal, or try to drill out as much as I can and use the cutter to clean it up?

              Comment


              • #8
                Originally posted by TRX
                .240 radius... .480 diameter. Arrrgh. I'm going to kick some dirt over that and pretend it didn't happen.

                Is a .110-.120 shank really enough to do the job? Should I make a clean cut into the metal, or try to drill out as much as I can and use the cutter to clean it up?
                I would rough it in with a unmodified #304 cutter and then finish with the one with the ground neck. Use lots of lube and go slow.

                Comment


                • #9
                  If you do it on the rotary table, the depth of the arc across the bottom would be about 0.0006". With the tolerance of 0.005" on the radius, wouldn't that be good enough?

                  Comment


                  • #10
                    I've printed out the drawing and using the 0.420" dimension and a good office metric rule got the scaling factor I needed and applied it to the 0.240" wood-ruff slot radius and I got 0.238" which verified the scaling factor and the drawing dimension.

                    No matter how you grind the woodruff cutter shank as the base of the slot is circular at some point you are going to have the cutter trying to cut the whole curve in the slot no matter if a standard width cutter is used or even if multiple thinner cutters are used and when it has no lateral movement to "play with" it may well try to "climb mill".

                    The width of the slot is not given so I will asuume it is either 0.094" (3/32") or 0.125" (1/8") and as the cutter radius is 0.240" its diameter is 0.480".

                    The nearest cutter is either a #304 or 404 which are 3/32 x 1/2 and 1/8 x 1/2

                    The cutter nominal diameters are 1/2" so they may need to be ground back to 0.480" (2 x 0.240").

                    http://www.metalwebnews.com/formulas...odruf-key.html

                    (Note the cutting depths)

                    http://www.google.com.au/#hl=en&gs_n...w=1280&bih=545
                    Last edited by oldtiffie; 05-26-2012, 10:34 PM.

                    Comment


                    • #11
                      Originally posted by oldtiffie
                      I've printed out the drawing and using the 0.420" dimension and a good office metric rule got the scaling factor I needed and applied it to the 0.240" wood-ruff slot radius and I got 0.238" which verified the scaling factor and the drawing dimension.

                      No matter how you grind the woodruff cutter shank as the base of the slot is circular at some point you are going to have the cutter trying to cut the whole curve in the slot no matter if a standard width cutter is used or even if multiple thinner cutters are used and when it has no lateral movement to "play with" it may well try to "climb mill".

                      The width of the slot is not given so I will asuume it is either 0.094" (3/32") or 0.125" (1/8") and as the cutter radius is 0.240" its diameter is 0.480".

                      The nearest cutter is either a #304 or 404 which are 3/32 x 1/2 and 1/8 x 1/2

                      The cutter nominal diameters are 1/2" so they may need to be ground back to 0.480" (2 x 0.240").

                      http://www.metalwebnews.com/formulas...odruf-key.html

                      (Note the cutting depths)

                      http://www.google.com.au/#hl=en&gs_n...w=1280&bih=545
                      The #304 cutter is usually supplied at .490" or slightly smaller. The width is .093. One pass with a roughing cutter and then two with the undersized neck to finish the width and depth. These are very light cuts with the finish tool. This is not brain surgery.

                      Comment


                      • #12
                        I would use a woodruff cutter and just do it. Look at it this way some one else did it so why can`t you. They had the same tools as you .If not you need some more tools.
                        Every Mans Work Is A Portrait of Him Self
                        http://sites.google.com/site/machinistsite/TWO-BUDDIES
                        http://s178.photobucket.com/user/lan...?sort=3&page=1

                        Comment


                        • #13
                          Originally posted by cameron
                          If you do it on the rotary table, the depth of the arc across the bottom would be about 0.0006". With the tolerance of 0.005" on the radius, wouldn't that be good enough?
                          I expect it would.

                          I come up with these occasional stupid questions when I look at something and wonder if there's some process out there that I don't know that I don't know, if that makes any sense.

                          Comment


                          • #14
                            Originally posted by lane
                            Look at it this way some one else did it so why can`t you. They had the same tools as you .If not you need some more tools.
                            This print is of the production part, which was intended to be an investment casting with minimum machining. I don't know if the slot was machined or used as-cast.

                            Width is .105 +/.005, -.000

                            correction: examining the print again, it doesn't actually say it's a casting. Since most of the other pieces are castings, I may have made an unwarranted assumption there. This just hasn't been my day for blueprint reading...
                            Last edited by TRX; 05-26-2012, 11:34 PM.

                            Comment


                            • #15
                              Originally posted by oldtiffie
                              I've printed out the drawing and using the 0.420" dimension and a good office metric rule got the scaling factor I needed and applied it to the 0.240" wood-ruff slot radius and I got 0.238" which verified the scaling factor and the drawing dimension.

                              No matter how you grind the woodruff cutter shank as the base of the slot is circular at some point you are going to have the cutter trying to cut the whole curve in the slot no matter if a standard width cutter is used or even if multiple thinner cutters are used and when it has no lateral movement to "play with" it may well try to "climb mill".

                              The width of the slot is not given so I will asuume it is either 0.094" (3/32") or 0.125" (1/8") and as the cutter radius is 0.240" its diameter is 0.480".

                              The nearest cutter is either a #304 or 404 which are 3/32 x 1/2 and 1/8 x 1/2

                              The cutter nominal diameters are 1/2" so they may need to be ground back to 0.480" (2 x 0.240").

                              http://www.metalwebnews.com/formulas...odruf-key.html

                              (Note the cutting depths)

                              http://www.google.com.au/#hl=en&gs_n...w=1280&bih=545

                              I think if he roughs it in with the standard #304 cutter he will have only .005" or .006" per side to take out. If he goes to .235" in depth with the roughing cutter he will only have .005" to finish it to full depth. The reduced neck cutter can certainly do this and produce an excellent finish whether or not you consider it climb milling. There is no climb or conventional about it. It is a simple in and out cut with very little material removal.

                              Comment

                              Working...
                              X