Center drills vs spot drills?

[Tom Szelag]

Whats the difference here. I'm well aware of what a center drill is and what its used for, but in some thread a while back regarding reaming holes someone was talking about how center drills weren't reliable enough.

 

Is the concept not the same? Have a short, stubby, rigid tool to start a straight hole such that a longer drill can follow it straight?

[5 AX]

Center drills are exactly that. They are for making centers. The smaller diameter tends to break off in the part during production use. This is not desireable.

[kinglouie V]

spot drills seem to be the culmination of the cnc

revolution in that a spot drill which has a much

stronger cross-section than a center drill will produce a spot for your drill in less time with more accuracy than a centerdrill due to it's increased rigidity. and to me they are much easier to program with respect to the size chamfer on the hole after drilling and tapping.

[robk]

Last time I've seen a center drill was in Mastercam's tool library

I haven't used one in years... You shouldn't center drill or spot drill for that matter prior to running solid carbide drills. We use spot drills for chamfering holes and contours.

[Psychomill]

+1 rob.

[Tom Szelag]

I get the feeling the shops on campus are behind the times then...always use center drills to start a hole (all our drills are HSS).

 

"We use spot drills for chamfering holes and contours."

 

So you use it as a chamfermill then, to break edges on countours?

[Tim Johnson]

Ok I'll start the controversy. With the understanding that the split point carb/short hss drills don't need the starting hole we have found here that the center drill is the more accurate spotting tool. The trick for holding the accuracy is NOT to use the same tool for chamfering. If your drill/reaming a 3/32" hole then use a No.0 center drill but only drill it to the chamfer. The idea is to keep the starting dia just barely bigger the the chisel edge/web of the drill. If the chamfer of the starting hole is bigger than the drill dia there is a tendency for the drill to pull. With the center drill starting dia into the part to the center chamfer there is also a guide to help hold the location.

 

This is my mnsho. What's yours?

[Mike Mattera - TFM]

I go with Kinglouie and Robk: Spot Drills for all holes. Mostly because of the champher, but also because of rigidity.

 

I have not used them for champhering contours but I dont see why not (in lighter alloys).

 

You can do most of your holes with a 1/2" and a 1.0" spot drill, instead of 4-5 different centering drills.

 

Mike Mattera

[Brendan P]

I don't like using a centerdrill that has a 60 degree included angle.

And then trying to follow that prestarted hole with a 118 or 120 deg. inc. drill.

[robk]

quote:

---

So you use it as a chamfermill then, to break edges on countours?

---

Sure do... Not sure how HSS would work, but solid carbide works great in 400 grade stainless. To be quite honest with you we use Harvey's carbide drill/end mill as our spot drills/smaller chamfer tools. The price is very good and you could drill (NOT steel) chamfer and mill all with the same tool. Works great on blending walls with chamfers.

[Psychomill]

I've used HSS coated and uncoated to chamfer in steels. Works fine. A little slower though...

[g huns]

Not to highjack this thread but since you mentioned Harvey(a big +1 to their spot/drill/chamfer tool) have you tried any of their thread mill cutters. Seem really cheap. I've been paying almost 3x what they are getting. Just wonderin.

[CAM-mando]

I am actually with Tim to some extent on this. For precision work, I prefer center drill (no chamfer tip only) then drill. I prep the hole with a separate c'sink as required.

 

That said, we should be using spot drills more than we do.

[robk]

I haven't tried them yet, but if they're as good as most of the other stuff they have than I will have to. This is the 1st time I actualy looked at their thread mills and they are very inexpensive... Now if only they could do a little better on the LOC for them.

[chopsley]

I've had good luck using Vermont Tool's "spott". It is a one insert indexable spot drill with a 144 degree included angle. That way it will nicely nest the point of any drill 140 degrees or less. This tool elimanates the need for resharpening so they repeat well. In most steels I run them at 1800 rpm .001. inch per rev. They can give you up to a .7 dia. chamfer. I use center drills mostly for shaft work where there are subsequent grinding operations.

[KJS]

Great Thread! My question is this, I'm drilling a .052 hole with a solid carbide drill and this hole has a pretty tight tolerance. If I can get a .053 gage pin in the hole the part is junk. How should I be starting the hole? With a small spot or center or nothing at all?

[5 AX]

I use harvey on a daily basis. The quality on everything they offer is amazing. I would recomend to anyone. I use the thread mill in titanium and I have not found anything that lasts longer.

[cblythe3d]

For best reesults your spot drill should have a equal or greater angle than your drill and if practical an equal or greater diameter.

 

The short rigid spot drill resists the tendancy to wander. The drill then contacts first at the tip and follows the spot location providing the best positional accuracy.

 

If you listen to a drill entering the hole left by a (lathe) center drill the nasty growling sound is the result of the external portion of the drill contacting first and jumping around. Bellmouth holes, drill damage, and loss of c/l position result especially when the surface is at an angle as in castings.

 

If the surface drilled is not perpendicular to the hole it is essential that the spot drill diameter is at least that of the drill.

 

Often in a production environment a 45 deg spotter will create the chamfer and guide the drill sufficiently saving a tool change. Worhs best with stub drills.

 

note: for best accuracy when gun drilling often the hole is spotted to the same diameter as the drill but sub flush leaving a guide bushing in the part.

[robk]

KJS, not knowing what drill you're using I will give you what works for us and what Mitsubishi recommends;

If using Micro MZS Drills;

If drilling a size less than 2mm(.0780") always use Micro MZE Pilot Drill going 1xD

High pressure pump (800 psi>)

Filter to 5 microns

Runout <.0003 max.

Coolant with E.P. Additives