No announcement yet.

metric conversion??????

  • Filter
  • Time
  • Show
Clear All
new posts

  • metric conversion??????

    Gentlemen, A customer wants me to drill and tap 5/16-18 every 4 inches o.c. for a depth of .440 for a length of 12 feet on 6 pieces of alum. 1.5x .5x 12. Not a problem on my Bridgeport, reposition quite a few times but an easy job. Come to find out he bought metric track; holes need to be 100 mm on center! What’s the best method with a lead screw that is .200 per revolution? Thanks

  • #2
    Buy a DRO with inch/metric coversion!

    A cheaper approach is to do a quick Excel spreadsheet or similar, to work out the dial numbers you'll get every 100mm. Since you want every 3.937", you'd have:

    (3)937 or a dial reading of 137
    (7)874 or a dial reading of 074
    (11)811 or a dial reading of 011

    You can get "pretty close" to where you want to be for each hole with a regular ruler, then worry about the last bit by setting the dial to 137, or 074, or whatever the table tells you.

    Or, a quicker way might be to make up a fixture with a locating pin, so you can drill the first hole, shift the work over until the pin drops in that hole, drill the next hole, etc.
    At least, that's how I'd do it.... It somewhat depends on what your tolerance is.

    [This message has been edited by SGW (edited 02-15-2003).]

    [This message has been edited by SGW (edited 02-15-2003).]
    Try to make a living, not a killing. -- Utah Phillips
    Don't believe everything you know. -- Bumper sticker
    Everybody is ignorant, only on different subjects. -- Will Rogers
    There are lots of people who mistake their imagination for their memory. - Josh Billings
    Law of Logical Argument - Anything is possible if you don't know what you are talking about.
    Don't own anything you have to feed or paint. - Hood River Blackie


    • #3
      Invest your effort into fabing a jig to locate each hole at a distance of 100mm (or whatever the job requires) from the previous hole. This could be as simple as a pin in a slip fit hole through any available bar scrap and clamped to the table. To set up the jig, chuck up the pin in the mill, advance the x axis 3.937", clamp the bar to the table and lock the table. With the worpiece either against a fence or held in a vice drill the first hole, slide it over and locate it with the pin and repeat aproximatly 36 times.


      • #4
        Dave has a good idea, but it reqires very careful manufacture for it to be effective.

        Either way, it is not a big deal. I would double check with him, the distance for the holes may not have changed even if he substitued metric material!


        • #5
          All good replies. I spent some time and worked out the spread sheet method, looks pretty easy. The jig looks easy to make also and a lot quicker to drill, but I wonder about accumulitave error after 12 feet? This track that bolts to the annodised and the spacing is dead-nuts on. I'm leaning towards the first method.


          • #6
            Cumulative error is indeed a concern in any operation like this. I think it’s wise to check with the client to ascertain what their requirements are. I would also strongly urge you to layout ALL of the hole locations in order to watch out for cumulative error (and brain farts).

            This type of situation has been a constant frustration to me over the years. I frequently encounter incorrectly dimensioned drawings created by people who do not understand the rules of dimensioning and tolerancing. This is a good example. Often these holes would be dimensioned showing “X holes 5/16â€‌ DIA, 100mm spacing typ(ical)â€‌. This would be an ideal situation for the jig I proposed since it is defining a distance between centers. BUT what is usually wanted and what should be drawn is X number of holes dimensioned from a common origin at 100mm increments. This may sound like the same thing, but if the machinist, toolmaker, or patternmaker lays the job out as drawn, the layout methods will be different and assuming the layout is not perfect but within given tolerances the resulting holes will not match up. In the first method the holes will be laid out 100mm from the preceding hole and any error will be cumulative. Assuming 10 holes and +/- .010â€‌ tolerance (Standard tooling tolerance for composite parts for a large American aircraft manufacturer) this could result in a cumulative error (also known as stacked tolerances) of .100â€‌. This part is probably not what was wanted and wont work, but it is within tolerance and is technically correct. In the second method each hole is laid out from a common origin resulting in a maximum error of .010â€‌ or .020â€‌ depending on whether the holes are dimensioned from the first hole in the sequence or from a common origin.

            I’m sure most of the pros and many of the hobbyists understand this, but I wish the engineers and draftsmen (and those training them) could understand the resulting differences.