Drilling Multiple Diameters.

[jheal2]

Hi.
When Drilling multiple holes on a lathe, all to different depths, is it always smallest hole to largest hole or is it sometimes beneficial to start with the larger holes first to save the smaller drill or for any other reasons (concentricity, finish, etc)

Thanks
Jordan

 

[MikeHalloran]

Because an ordinary two-flute twist drill is stabilized by the chisel point between the flutes, after spotting a center, I'd start with the large hole, then proceed to drill smaller holes in that order, large to small.
... That's how I'd program it for CNC, to maximize metal removal rate, and not expend any effort or time drilling through material that I was going to remove later anyway.

However, when I work on a lathe by hand, I almost never do it that way; I start with the small hole and work up to the larger ones.



Mike Halloran
Pembroke Pines, FL, USA

 

[saberblue]

If you are doing any volume at all make or have someone make for you a "step drill". This is a multi diameter drill that will do all the holes in one pass. If the drill is made properly it will take care of the concentricity -- however because you will be drilling all the diameters at one RPM (SFPM) if there is a large difference in the diameters you may have surface finish problems

 

[jheal2]

Saber, we do use step drills for alot of applications, this was for all of the times without. Thanks though.
Mike, this is opposite to how I would have done it, trying to reduce how much force that I need to push the drills through, but that is like you said the manual way of thinking and your logic makes complete sense as well. I have made parts manually, and ran CNC's for a long time and now I am taking a hand at programming CNC's. Thanks for the input.
Jordan

 

[saberblue]

It seems to me that the order you choose to drill in is going to be very much a question of how badly/easily that he material being drilled work hardens

 

[BillPSU]

You should really step back and look at what you are doing. If you are using a twist drill or an inserted drill what forces are being generated. In a twist drill or spade drill application the maximum forces are generated supplying thrust for the drill while an inserted drill requires spindle horsepower. If your thrust capabilities is sufficient for the large twist or spade drill then do the large hole first if the thrust capability is insufficient then use the small drill first to reduce the thrust required otherwise you will have axis following error and possible overload of drive systems and even the structures of the machine. Inserted drills need coolant through the tool to help blow the chips out and cool the cutting tool. If you don't have the ability to deliver coolant with sufficient flow rate and pressure insert drills have been known to be terrific friction welding devices.

Look at each application and choose you method but then be willing to change if problems occur.

 

[jheal2]

Hmm, never really took into account the power behind my axis's and spindle. I dont believe that any of our parts will be a problem because most holes are smaller than 3/4" but if any larger jobs come up this will be definately be handy information.
Thanks Bill

Jordan

 

[MRSSPOCK]

I haven't heard any mention of tolerances so far. That's also got to be a considerable factor. Depending on tolerances, your penultimate drill might be the centre drill again.

 

[MRSSPOCK]

i.e. if you start off with the big Ø

 

[jheal2]

Hi MRSSPOCK
Again, I didnt have a specific part in mind but tolerances usually run from about .002 to .010 total depending on the part. So not overly tight, some more than others.
That was also my train of thought using 1 centre drill for the first drill and none after that. But wouldnt this work both ways?
Big drill first and you have the existing drill point to use.
Small drill first and you have the existing hole to use.
That is of course if the first drill was not wandering.

Thanks
Jordan

 

[MRSSPOCK]

Regarding your last comment, hole depth then becomes a factor as well. Let's say you have a Ø1" hole X 6" deep, stepping down to Ø1/4" X 1" deep, you might find it difficult getting back in to centre drill again. However you really can't expect to rely on the Ø1" drill point to leave a nice face for the Ø1/4" drill to start on. So, I think it all boils down to doing what is practical for any given situation.

 

[WelshWizards]

depending on the smallest bore have you considered a stepped and piloted core drill that can run of the smallest diameter, a well made stepped core of either three or five flutes should give good stock removal as well as a reasonable finish, and if the small bore requires a good finish drill about .015" small and then finish with a reamer to size.