measuring small holes

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • mdred68
    Member
    • Sep 2005
    • 56

    measuring small holes

    I have a job where i have to machine 12 holes .190" + or - .001 at a depth of .015" + or - .002 how do i measure these accuratly. I dont think dial calipers are the right tool for the job. Thanks
  • darryl
    Senior Member
    • Jan 2003
    • 14419

    #2
    That's not very deep- more like a decorative mark. That's also a pretty close spec to rely on a drill to make the holes. If you need to measure to be sure the hole is on diameter, you could turn a short stub on some round bar to the size you want, then use that as a gauge. Maybe make two or three of these 'test stubs'- one a tad small, one right on, and one a tad large.

    If the problem is getting the hole to be the right size, it might boil down to you having to make a custom drill bit, which you could then incrementally grind narrower until it drills the hole the exact size you're looking for. I'm thinking this would be more of a spade bit than a drill bit in the conventional sense.

    The shallow depth would seem to me to make the hole difficult to use, and it has me wondering if the spec is just a spec and not a hard requirement. Maybe you just need to make sure that all holes you make are the same diameter and depth, and not necessarily an exact size- if so you can make up a tube to slip over the drill bit to act as a stop. You can also drill the size hole in a strip of steel, which you then use along with the spacer tube on the drill bit. The strip of steel takes the polishing from the spacer tube and you can avoid marking up the workpiece.

    I'm probably going off on a tangent without more info-
    I seldom do anything within the scope of logical reason and calculated cost/benefit, etc- I'm following my passion-

    Comment

    • Machinist-Guide
      Senior Member
      • Nov 2009
      • 245

      #3
      .190 hole

      + or - .001 = .002 tolerance so I am thinking calipers would be O.K. At .015 depth I would call this a spot face rather than a hole try plunging a 3/16 center cutting endmill. The endmill it's self is .187. Considering spindle run out and endmill wobble caused by plunging you just may end up with a .190 hole. As for the depth I would use depth mics.
      Last edited by Machinist-Guide; 02-01-2011, 08:44 PM.
      Visit my site for machinist videos free charts & more

      Machinist Classifieds Free Listing

      Comment

      • Toolguy
        Senior Member
        • Jan 2010
        • 6669

        #4
        Small Holes

        The best way to measure something like that is with gage pins. As for making the holes, If you have CNC, use a 1/8" end mill and do a pocket routine. Then you can adjust the size of the hole with the program and make them all right on the money. If you only have manual, you could plunge with a 3/16 end mill, 4 flute, and maybe get it that way. An end mill always cuts oversize in a drilling application. Deburr and depth mike as stated above.
        Kansas City area

        Comment

        • randyc
          Senior Member
          • Jun 2003
          • 460

          #5
          Originally posted by Machinist-Guide
          + or - .001 = .002 tolerance so I am thinking calipers would be O.K. At .015 depth I would call this a spot face rather than a hole try plunging a 3/16 center cutting endmill. The endmill it's self is .187. Considering spindle run out and endmill wobble caused by plunging you just may end up with a .190 hole. As for the depth I would use depth mics.
          I agree and if the hole isn't quite .190, slip a scrap of cellophane (or "cigarette paper") along one side of the end mill shank before tightening the collet (to offset it slightly) - adjust the thickness as required to fall within the middle of the tolerance range.

          I don't see this as a serious measurement problem and would use calipers for depth determination as well. The only problem with the end mill is whether the spotface needs to be flat-bottomed. Most center-cutting, two-fluted cutters are slightly angled.

          Comment

          • Dan Dubeau
            Senior Member
            • Dec 2008
            • 4381

            #6
            Originally posted by Toolguy
            The best way to measure something like that is with gage pins. As for making the holes, If you have CNC, use a 1/8" end mill and do a pocket routine. Then you can adjust the size of the hole with the program and make them all right on the money. If you only have manual, you could plunge with a 3/16 end mill, 4 flute, and maybe get it that way. An end mill always cuts oversize in a drilling application. Deburr and depth mike as stated above.
            +1 to everything. Play around with some scrap to figure out what a 3/16" EM will cut your hole at, then shim it over in the collet, or play with speeds, and feedrate to get it within tolerance.

            As for measuring, if you don't have a set of pin gauges, you can make a pretty simple go/nogo gauge out of drill rod. Just turn one end to 0.1910" (+0/-0.0001) and the other 0.1890" (+0.0001"/-0). If you have a lathe the job it pretty easy, if you have a surface grinder and a spin fixture it's even easier. Depth mic for depth.

            How is your customer going to measure these holes? CMM? calipers? pin gauges? hole gauges? calibrated eyeball? If they are just going to slap a caliper on there and call it good, then thats exactly what I would do and call it a day. If they are going to check them via more accurate means, then it's time to do the same. Find out what they use to measure them, and emulate it.

            Comment

            • srednalf
              Junior Member
              • Jan 2011
              • 8

              #7
              Buy a small set of reamers in the area of the size you need. Use one that is smaller than you require and let it ream the hole to the max that it can, and measure with gauge pins. Then step up in ream size. Remember, the longer you let the ream work the hole, the more material you take. So patients can get you to perfection. Use oil, and move the reamer up and down slowly on low rpm. It sounds like the customer is intending to place dowel pins for location purposes. Depth is probably not as important,but lust in case it is,.. Drill the hole approx .30 Undersized, then use a flat bottom end mill also .30 undersized and create a flat bottom inside the hole to allow for a depth gauge. Be sure to establish depth before diameter. Find out about depth. if you can go a little deeper, you can nail the diameter easier.

              Comment

              • JCD
                Senior Member
                • Feb 2005
                • 246

                #8
                A Starrett Small Hole Gage 830B would work nicely.

                Comment

                • Ryobiguy
                  Senior Member
                  • Sep 2003
                  • 366

                  #9
                  Originally posted by srednalf
                  Drill the hole approx .30 Undersized, then use a flat bottom end mill also .30 undersized and create a flat bottom inside the hole to allow for a depth gauge.
                  How can you can drill a .190" diameter hole undersized by .30? Are you talking .30mm maybe?

                  -Matt

                  Comment

                  • Mcgyver
                    Senior Member
                    • Mar 2005
                    • 13409

                    #10
                    Originally posted by srednalf
                    Buy a small set of reamers in the area of the size you need. .
                    I like the idea of a reamer, but might be tough do for this depth - whats the bottom of the hole look like; is drill point ok or does it have to be flat? Do get to spot drill it? or is a pilot ok? Small pilot followed by a homemade counterbore would do the trick.

                    Remember, the longer you let the ream work the hole, the more material you take.
                    that I haven't heard before....reamers cut at the end, so how does that work? Can't see it frankly.

                    For measurement, use pin gauges if you have them or turn a go/no go gauge. I wouldn't think calipers at that tolerance, heck you could get 1/2 a thou or more error because of the flats on the points when measuring a small bore like that - you're only +- .001 and on top of that have figure calipers are shaking at being better than a thou.....but I like the idea of querying the customer of how they'll inspect; might smoke out some BS
                    located in Toronto Ontario

                    Comment

                    • srednalf
                      Junior Member
                      • Jan 2011
                      • 8

                      #11
                      Yes, if you continue to run a reamer it will go slightly above it's measured size, (If the reamer is new, or freshly ground) All steel tools wear, so determining the depth allowance. is good if you can go a bit deeper as to allow for wear on the tip of a used reamer. Reamers do not only cut at the tip. You use the entire reamer or the part of it that you find will do the job In precision work. I'm talkin .0001 and less. Next step up would be jig grinding.
                      I've built hundreds of plastic injection molds. Precision is my game. Thousands of cores built within .0001 tolerance so you learn a few things that you might not normally try. If these holes are for dowel pins to connect to parts in precision locations the location is just as important as the hole size. If this was high precision, The customer would have requested jig grinding of the holes.

                      Comment

                      • srednalf
                        Junior Member
                        • Jan 2011
                        • 8

                        #12
                        Originally posted by Ryobiguy
                        How can you can drill a .190" diameter hole undersized by .30? Are you talking .30mm maybe?

                        -Matt
                        Use a .160 drill.....A #20 drill is.161

                        Comment

                        • Toolguy
                          Senior Member
                          • Jan 2010
                          • 6669

                          #13
                          Small Holes

                          These holes are only .015 deep +or- .002. You're not doing that with a reamer.
                          Reamers have a 45 degree bevel on the end and they are not center cutting.
                          Kansas City area

                          Comment

                          • Mcgyver
                            Senior Member
                            • Mar 2005
                            • 13409

                            #14
                            Originally posted by Toolguy
                            These holes are only .015 deep +or- .002. You're not doing that with a reamer.
                            Reamers have a 45 degree bevel on the end and they are not center cutting.
                            Depends on the shape of the bottom....could be a .015 deep hole with a 118 point which case you'd drill as close as you could, say # 13, then ream the last couple of thou and it would work and be on spec....hey, my mind went to a flat bottom hole too...but we don't know that.
                            located in Toronto Ontario

                            Comment

                            • randyc
                              Senior Member
                              • Jun 2003
                              • 460

                              #15
                              Originally posted by Mcgyver
                              ... I wouldn't think calipers at that tolerance, heck you could get 1/2 a thou or more error because of the flats on the points when measuring a small bore like that ...
                              Excellent point and one that I overlooked - the error on the first pair of calipers that I picked up was actually .002 when measuring a .190 diameter bore. However the error is consistent and can be accounted for in the measurement by adding .002 to the dial reading.

                              I don't trust many forms of measurement in a hole this shallow, gage pins for example or inside micrometers (if a pair can be found that will measure under .200 diameter). I have a pair of older style vernier calipers with a ground, rounded shape that gets around that problem but they are also limited to .200 minimum diameter.

                              Comment

                              Working...
                              X