Announcement

Collapse
No announcement yet.

Need to make 24 of these

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

  • Need to make 24 of these

    Looking for some advise from those in the know. I need to make 24 of these out of 6061. I will cut the 5 inch long 3 inch cylinders on my bandsaw and face them on the lathe. This will be the first time I will make money on anything. Everything else in the past has always been free or for buds of mine. Any machining tips, tooling, machining the pockets, setup, jig etc., help would be greatly apprecaited to cut my time. I have a EMCO Maximat v10 and an old Bridgeport. I don't mind buying tooling if it saves time.

    http://www.pbase.com/smokedaddy/image/107221651

    Thanks in advance,
    -SD:

  • #2
    how to go about it has everything to do with tolerances. For example off far off concentric can the bores be from the cylinder for example, do the counter bores have to be flat, how concentric do they have to be, how much wander is permissible with hole etc.

    I'd consider getting the service centre to chop them to length. they'll have a blade with enough tpi for 3" stock, us home shop guys usually don't. you save time and probably money as their big saw will make very square cuts where as you have a cheapo with high tpi it can wander more easily - that uses more material. that and get a bunch of different quotes, service centre pricing depends on moon phases it seems. they'll budget a 1/8" saw kerf - are you going to be able to hold to that on your saw?
    .

    Comment


    • #3
      Whats the part do?
      This product has been determined by the state of California to cause permanent irreversible death. This statement may or may not be recognized as valid by all states.
      Heirs of an old war/that's what we've become Inheriting troubles I'm mentally numb
      Plastic Operators Dot Com

      Comment


      • #4
        That's very cool! How you gonna weld them little pipes in there?
        Sorry..I just had too...
        I have tools I don't even know I own...

        Comment


        • #5
          1/4 inch bore

          I would be concerned with the 3 inch long 1/4 inch bore. Does it have to be concentric to the counter bore on each end? A long 1/4 bit can be pretty flexible. Or even worse are they a reamed hole that is concentric? Is the tolerence indicated by the drawing the desired tolerence?

          Comment


          • #6
            I was asked to make one so they can see if it works, then make the others. The bores need to accept a piece of 1.625" copper tube. A tolerance wasn't given to me, probably 3 thousands? It needs to fit just like a piece of 1.625" copper tube would in a 1.625" copper fitting, like a 90 degree elbow for example. Concentricity isn't that critical, nor is the perpendicular bore. The bottoms need to be flat but the flatness isn't critical either. The .25" bore isn't critical either, it is just for a argon gas purge. I think my bandsaw cuts pretty accurate but I will ask about the cost of pre-cut pieces.

            http://www.pbase.com/smokedaddy/image/107223418

            Any suggestions are appreciated, tooling, cutting the bores etc.

            Regards,
            -SD:
            Last edited by Smokedaddy; 12-18-2008, 10:17 PM.

            Comment


            • #7
              SD,
              For the cutoffs I would use a 4 tpi skip tooth blade. Pick the shortest one then:

              In the lathe: (assuming a QCTP)
              Face one end, break edge, 45* angle for chamfer.
              With a cheap turret tailstock:
              Spot drill
              pilot drill 3/16", 1.5" deep
              drill 1 1/4" 1" deep from touch
              Set saddle stop
              Bore to size, one rough cut, two finish cut to size.
              with the turret, drill 1/4" to 2.5" depth
              Return facing tool, cham bored and drilled holes.
              repeat.
              THEN do the other ends.

              In the mill:
              set an end stop on the vise
              place first part in mill vise
              MAKE SURE boring bar and all tools fit in the vertical space.
              find center
              Spot drill
              1/4" to intersect
              1 1/4" to depth
              Bore to size.

              This is based on my machines, and my style, YMMV.
              Dave J.

              Comment


              • #8
                Dave,

                Do they make a 1 1/4 bit for a #3 Morse Taper (I think that's what mine is)? I haven't a clue as I've never bought a morse taper bit. Or I assume I would need to buy a bit with a turned down shank. Think my lathe can handle a bit that large? Sure would be nice.

                http://www.pbase.com/smokedaddy/image/107227294

                http://www.pbase.com/smokedaddy/image/107227292

                Oh, and how would I make the bottom of the bore flat (if that's what they want)? It doesn't have to be perfect, just aesthetically pleasing.

                -SD:
                Last edited by Smokedaddy; 12-19-2008, 12:36 AM.

                Comment


                • #9
                  parts

                  SD,

                  MT for a drill bit, ouch !
                  I have a 9x20 and used a 1-15/32 bit in some Al. today, not a problem.
                  The bit had a 1/2" shank on it in a MT2 drill chuck. Just get one close to the size you need, get as much of the hole as you can with the bit, then usea boring bar to flatten it out and get the ID right. Much cheaper than a MT bit IMO.
                  My metal man has a cnc saw, and could cut your stock to your lengths in a few minutes. Cheaper if you don't have the time to DIY. Expensive if you do have the time. Oh, if you do have it cut somewhere, make CERTAIN you spec enough length for each piece to face the ends to the right length. For example: If you tell them 6- one inch pieces out of a 6" round, Al., they give you just that. When you have to face it on the lathe, you can have from .850-1.003" finished thickness unless you specify.

                  Make sure to specify if you have them cut it for ya.

                  If you have a small 4x6 bandsaw, you can order a 6 tpi blade ( or was it 5 tpi) for it for cutting larger diameter Al. rounds. Works like a charm, much faster cutting. ( I got me one of them ! )

                  FWIW
                  Lenord

                  Comment


                  • #10
                    For the flat-bottomed hole, can you find a 1 1/4" end mill (or slot drill) on a 3MT? Use it to finish the hole to size and leave a flattish bottom in one pass. End mills are ground with a very slight fishtail, but it doesn't sound as if this would be a problem in this case.

                    Ian
                    All of the gear, no idea...

                    Comment


                    • #11
                      I don't know your customer but I'd make them tolerance the thing before committing to it or at least sign off on the tolerances you decide you want to hold. . .

                      The nice thing about doing things for ourselves and buddies is that we know what will work and can relax tolerances as progress on the part dictates.

                      In the mold I recently made, one of the end plates is short by .120 in the x dimension because that is what it took to clean up some out of square sawing done by the service center.

                      If this was a paying job, the part would have to be scrapped and I'd be over at Crucible complaining. On the other hand, since it was for me and a one-off I just made sure to chose x so that that side would not be on the bottom which would keep the part from sitting up as needed.

                      --Cameron

                      Comment


                      • #12
                        Originally posted by lenord
                        SD,

                        MT for a drill bit, ouch !
                        I have a 9x20 and used a 1-15/32 bit in some Al. today, not a problem.
                        The bit had a 1/2" shank on it in a MT2 drill chuck. Just get one close to the size you need, get as much of the hole as you can with the bit, then usea boring bar to flatten it out and get the ID right. Much cheaper than a MT bit IMO.
                        My metal man has a cnc saw, and could cut your stock to your lengths in a few minutes. Cheaper if you don't have the time to DIY. Expensive if you do have the time. Oh, if you do have it cut somewhere, make CERTAIN you spec enough length for each piece to face the ends to the right length. For example: If you tell them 6- one inch pieces out of a 6" round, Al., they give you just that. When you have to face it on the lathe, you can have from .850-1.003" finished thickness unless you specify.

                        Make sure to specify if you have them cut it for ya.

                        If you have a small 4x6 bandsaw, you can order a 6 tpi blade ( or was it 5 tpi) for it for cutting larger diameter Al. rounds. Works like a charm, much faster cutting. ( I got me one of them ! )

                        FWIW
                        Lenord
                        MT is normal for accurate drilling and essential for large diameter- most of my 13mm+ is MT and a fair amount of the less than 13mm that I use for close tolerance work. you can get a 1 to 1.5" cheap on Ebay in the UK £10, $15.
                        I suggest you work up the operations you want to do assess the tolerances you can work to and then give them a marked up drawing with what you want/can to deliver...
                        e.g. that you only need a flat in the bottom of each bore is 1.2 times or greater than the thickness of the tube and the remainder can be conical. and that the bore 1.6" bore is -0+0.010 and all other dimensions are +/- 0.010.


                        If the tubes are glued or soldered in this should be fine.
                        The description of the application seems that close tolerances are not required. Sending a marked up drawing will make that certain.
                        Last edited by derekm; 12-19-2008, 08:41 AM.

                        Comment


                        • #13
                          my question would be to you guys that know what your doing. . . .
                          how long would it take to make just one ? ? ?

                          10 minutes ?

                          30 minutes ?

                          after you had the stock sawed and in your hand.

                          hunting around for the tools after you start is a real pita then finding your drill is dull or whatever. . .

                          what would be the chance of the small hole being drilled from each end, actually aligning decently if it were done that way ?

                          for purging a gas, i would think the bottom of the hole would be better it not flat but tapered about the same as the drill point.

                          humm. anyone ???

                          Comment


                          • #14
                            If the bottom of the hole has no function I would drill with 1 7/16 dia drill and bore to 1.5 leaving a small flat bottom lip for the pipe to register on. Of course discuss this with the customer beforehand.

                            Comment


                            • #15
                              After all parts are faced to length I would do all operations by Mill, Using Horizontal/Vert. V-Jaws on my vise I would center drill and drill the two end 1/4" to intersect and then endmill and bore to size, set up stop and repeat for 90 degree intersect for both the 1/4" and then endmill and bore.

                              Comment

                              Working...
                              X