Post By dstryr
Post By Gary E
Post By scadvice
Is a drill going to give me a straight hole?
I am going to make some parts out of hot rolled steel blocks 3.25 x 3.6 x 4.144 in.there is a 8 hole pattern, they are all THRU holes, 6 holes are called out to to the center on the top of block, 2 called out to the center of part on bottom of block ,they get reamed. I want to drill all 8 holes from the top, flip the part and ream the two on the bottom. What I am worried about is the holes moving by the time I get to the bottom, I am using a .484 drill 5in. l.o.f and drilling to a depth of 3.75 in. Will my hole location change by the time I get to the bottom of part 3.6in. thick? I have a tolerance of +/- .001 on all hole locations.
Drill those 2 holes a little smaller,then flip and bore?
I would shoot for the following althought +/- .001 on a drilled hole 3.75dp is going to be a bitch....
Circle hole with em or bore a perfectly straight pilot
Drill with stubby drill
Drill with longer drill
All from one side. The error just from loading the other side will make your +/- .001 out of tolerance...
If your customer does not have much in inspection equipment then you can probably blast it with a jobber drill using a reasonable spec and conservative speeds and feeds. If they have a whiz bang 0.0000002 inch cmm you as they say are toast. Myself, if I had many of them to do I'd gundrill it in the vmc but I am set up for that, would just have to get the drill. It helps if you know how the guy writing the check is paying for it. You may be able to recover if they give you +/- 0.010 on hole size and end up inside of a workable cone... but if they spec +/-0.001 on the hole diameter then you need to think the matter through.
My bet is you wont hold the +/- 0.001
And since I have no clue what Jig Boring Machine you are going to use, I'd even lay odds to it.
NOW... before you do anything with what ever you call a reamer...
GOOGLE ..... JIG BORE Reamers.... READ about them
I'm using a fadal vmc, I have to ream holes to .501 1.in. depth after drilling .w/ .484 The parts are for a double drilling machine for in house use, so I don't think they are going to check on cmm. I know I'm not going to hold .001 tol., but I would like to be as close as possible, and as of now all I have is a hss .484 drill.
Originally Posted by Gary E
Do you have CTS? Guhring (and a few others) makes a drill that will blast those hole, on size, decent finish and straight. But for a depth like that, they make a 140° spotting drill to make sure the drill starts out straight.
If you still can't get it done, I'm just across town
+1 on doing everything from one side.
Each hole should be spotted, predrilled, drilled and reamed EXACLY the same way.
No flipping or turning or playing with speeds/feeds. Dial those in on a test block before scrapping the part.
Each of the above will change the way your drill aligns in the hole.
Believe it or not, your machine WILL bend in all directions as it drills.
Also beware that when there is a thin wall on one side of a hole, the drill will try to wonder that way.(sometimes 90 deg along the wall though)
Not sure if its linked to the density of the material or heat transfer but it will deviate.
Drills are kind of like a hatchet, they pretty much just move metal, they are floppy, especially on long length and aren't particularly accurate.
I can't think of a better way to punch a hole through metal, then.. well.. a punch.
Reamers are cool as hell too, They make holes that are pretty damn round, on size, generally a pretty good surface finish, but they too, are
floppy and just follow the hole you stuff them down.
So you already have a way to punch the hole (drill) and a way to size the hole (reamer). What you don't have is a way to straighten the hole.
The reamer is not going to do that, even chucked up short a rigid, they just aren't made for it.
You do have a drill, that's probably not going to make a straight hole. There are ways to maximize your drills ability to drill straight though.
A drill can drill pretty damn fast, but that's a lot of pressure, I've found if fed light to moderate, you've got a better chance of making a
straight hole. A pilot drill, sized between the web thickness and 1/3 the diameter of the drill helps, gets rid of the zero surface speed thing
where the drill is pretty much wiping instead of cutting.
You can start with a stubby drill, those drill a bit straighter than one hanging out 10X D. Not as floppy.
You could come in with something under your .484 for 3/4 of an inch or so deep, then bore or interpolate a pilot at the size of your
.484 drill. Now your drill has something straight and in position to guide it.
Looking again here, do what you can to keep your holes straight, then on your second side, drop a 1/4" endmill in, and interpolate yourself out to
.492 or so, then ream.
Punching a hole that is clearance for a bolt, not a biggie, on size, straight, on position holes, not a hole hell of a lot of fun, its really boring. Probably
about the crappiest feature you will ever have to do, and those damn engineers keep putting crap like that on parts, so you keep having to do them
over and over and over again.
Drill full depth around 1/64 th undersize...take a boring head and line bore about two diameters deep almost to size say .002 or less undersize. Ream for here to size. This will keep you about as straight and to true position as you can expect to get. I would say close to what your after...well at least best effort. The bored hole acts like a guide bushing positioning the reamer and should re-aline the drilled hole.
Originally Posted by Bobw
Well I took your advice, for the most part. For the the 2 holes in question I center drilled then used a .409 stubby carbide, went 1.5in. deep, then interpolated to .484 1.505in. deep, then center drilled again, then drilled thru with the .484. After all holes were done flipped part spun the holes and reamed. It might have been overkill, but I somewhat checked location by indicating 4 holes on bottom and by my figuring I should actually be in
tolerance. Thanks for the help.