Announcement

Collapse
No announcement yet.

All the gear and no idea :)

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

  • All the gear and no idea :)

    Ok, so i have converted to CNC on my Bridgeport

    I want to make these parts as part of an attachment that will allow me to mount my high speed spindle to the quill of the BP.

    My issue is that i have no idea how to go about mounting and what order to machine the features in?

    I have vague ideas but nothing thats telling me "thats how it will work" etc.

    How would you guys tackle this??





    Part is too big for my vise and there is +2-3mm all round to come off the profile.

    Material is Aluminium, 15mm thick.
    Last edited by Davek0974; 08-31-2016, 05:02 AM.
    If it does'nt fit, hit it.
    https://ddmetalproducts.co.uk
    http://www.davekearley.co.uk

  • #2
    Print out 1:1, and lay on top (or spray glue) of stock to pop center point for big holes. Drill some clearance holes for 1/2" hold downs (I'm assuming the smaller hole in the bottom part is larger than 1/2"? if not use smaller bolt). Now bolt it down through those holes, and cut the outside profile, and center groove/holes. While it's still bolted down, clamp it down from the outside in a spot where you wont nail the clamps while milling the rest. Set your Z 0.005" off the table, and you won't hit it. The 5 thou no cut will be cleaned up with an edge break later. Alternativly you could put a peice of paper between the part and table, and cut into that. The pinch bolt holes can be done in a vice, and the slots either with a slitting saw in that setup, or with a bandsaw/hacksaw (they're just slots.....) as the last step.

    Edit: Just noticed you're a Brit......use 12mm hold downs....
    Last edited by Dan Dubeau; 08-31-2016, 09:08 AM.

    Comment


    • #3
      Sounds good, i'm universal so 1/2" or 12mm its all good

      Would something like this get a chamfer or not?

      I have plenty of experience in manual stuff on the BP but very little knowledge so far of CNC - it opens up so much that i did not realise I had no clue about Even simple stuff like the chamfer - i wouldn't have even tried that manually, the ends would have been done on a rotary table etc.

      Mill pockets and drill for the pinch bolts before cutting the slots or after, they can be quite large so was thinking of using a 5mm slot drill on the slots.

      The drills need to breakthrough so rather than the paper spacer i would likely go for some sacrificial scrap, i have plenty of 3mm stuff and some 10mm junk.

      Edit....

      Just thought, if i have cut the mid slot and drilled the three holes then changed clamps and cut the two big holes, how would i flip it over and add the three counter-bores? I need to pick up a datum again from something?

      Or would it be best/accurate enough to do the inside features as above but then flip/realign on the raw stock edges as before then do the counterbores followed by the outside as the last process?
      Last edited by Davek0974; 08-31-2016, 09:20 AM.
      If it does'nt fit, hit it.
      https://ddmetalproducts.co.uk
      http://www.davekearley.co.uk

      Comment


      • #4
        Maybe better....

        Align and rough-clamp the blank then put the three counterbores in first, flip over, realign, then add all the other features and profile - the counterbores are the least important feature so a 1/4 or 1/2mm variation would not matter.
        If it does'nt fit, hit it.
        https://ddmetalproducts.co.uk
        http://www.davekearley.co.uk

        Comment


        • #5
          Originally posted by Davek0974 View Post
          Would something like this get a chamfer or not?
          With CNC, you can do lots of things you would not think of doing manually. For example, you can chamfer using a countersink or even a 90 degree spot drill.

          Originally posted by Davek0974 View Post
          Mill pockets and drill for the pinch bolts before cutting the slots or after
          Consider circular interpolation for the holes and counterbores instead of drilling. No need for a pointy drill to break through. If you do not have an auto-toolchanger or something like the Tormach system, try to minimise the number of tools you use. Each time you change, you have to reset the Z.

          Originally posted by Davek0974 View Post
          Just thought, if I have cut the mid slot and drilled the three holes then changed clamps and cut the two big holes, how would I flip it over and add the three counter-bores? I need to pick up a datum again from something?
          Put a sacrificial piece on the table under the part. Once the first operation is done, remove the part and mill out the two big holes again but the other side of the line (i.e. two bosses sticking up). Relocate the main part over these. Alternatively, mill a pocket the shape of the outside contour into the sacrificial plate. Use this to relocate. Pocket only needs to be 2-3mm deep. Sacrifical piece does not have to be metal - could be MDF or plastic.

          I would pick the biggest tool that can fit in the two end slots and do the whole thing with that one tool.

          Something wrong with the CAD model as it shows a different object upside down to right way up.

          Comment


          • #6
            Great stuff, thanks,

            I have repeatable tooling so no need to measure the Z again, it's all in the tool offset table

            The cad is correct ( i think ) it shows the bottom and top plate of what will be an H on its side when finished, the bridge piece is not shown. The small hole has a stub in it that will locate into an R8 collet, the larger hole in the top plate will clamp round the quill and the two holes on the right will clamp the spindle motor.

            Thats the plan anyway.
            If it does'nt fit, hit it.
            https://ddmetalproducts.co.uk
            http://www.davekearley.co.uk

            Comment


            • #7
              Originally posted by Davek0974 View Post
              The cad is correct (I think) it shows the bottom and top plate
              Sorry. I thought the drawings were two views (top and underside) of the same part.

              There are actually two parts. This is a very good reason to mill a pocket into a sacrificial piece and use as a fixture.

              You could mill a T-shaped slot (very long head and short shaft) into the pocket that would help locate the pieces when turned on their sides for the cross holes and counterbores. If you are really smart, the pocket in your fixture plate could be extended to incorporate the shape of the angle plate used to support the pieces when turned on their side.

              I do not know how critical the two big bores are (sounds like they are for clamping onto something) but if very important you can rough them out with circular interpolation a little small and then single point finish bore them as a later operation. This eliminates the effects of any backlash in your setup.

              Comment


              • #8
                If this is one each I wouldn't bother with a fixture of any kind. I always have a sacrificial aluminum tapped plate for the machine. Every so often you take 5 thousands off to remove the marks, drill divots don't matter. I'd likely drill and counterbore the clamp holes first while the part is stiff. Then lay it down and cut all the interior features while clamping on the four corners. Then reposition two clamps onto one side, and remove the other two. Profile the open side. Put the clamps on the profiled side, remove the other two and finish cutting it out.
                Alternately a Kurt style vise with aluminum soft jaws with a step. Use an end stop, clamp it up on edge, drill and counterbore, cut to width. Then lay it in the steps and clamp it, and finish, cutting right into the softjaws to do the curves on both ends. I have lots of soft jaws, take a bit off the top, cut it for the part and go.

                Comment


                • #9
                  Years ago I picked up a cast iron spindle arm from Tormach for pretty cheap, I think they were less then $50, finally used it to mount one of my NSK spindles to my mill. You might see is they still have them, you really want cast iron to dampen any vibrations.

                  Untitled by Jerry Biehler, on Flickr

                  Comment


                  • #10
                    Thanks all, I have started on these now,

                    In the end i opted to do the outer faces first, two 13mm holes were bored at the centres of the two final holes, the counterbores were added and then the part was flipped over, bolted through the two holes on sacrificial scraps, aligned with the axes and the perimeter was finished.

                    Next i will fit some clamps to the outside, remove the bolts and machine all the internal features.

                    This should keep the accuracy where its needed, any minor variation will be in the counterbores which are not critical.

                    Thats a nice spindle but i doubt the tormach arm would fit a Bridgeport or my water-cooled spindle?

                    Dave
                    If it does'nt fit, hit it.
                    https://ddmetalproducts.co.uk
                    http://www.davekearley.co.uk

                    Comment


                    • #11
                      The arm fits a standard 3-3/8 quill. My mill is bigger than a standard Bridgeport, it's equivalent to a series II. It should hold one of those spindles fine and its cast iron which should help dampen vibrations.

                      Comment


                      • #12
                        Fits like a glove



                        Should work nicely, very firm, no vibrations.
                        If it does'nt fit, hit it.
                        https://ddmetalproducts.co.uk
                        http://www.davekearley.co.uk

                        Comment

                        Working...
                        X