Thread: advice on drilling as cast holes in aluminium casting

hi,
We need to drill as cast holes7mm dia to dia 8.5mm and tap them to M10 , which is the best way to avoid drill them without drill drag.

advice
thanks
rags

Plunge an end mill that size. If additional depth is required, follow with same size drill.

Originally Posted by rags

hi,
We need to drill as cast holes7mm dia to dia 8.5mm and tap them to M10 , which is the best way to avoid drill them without drill drag.

advice
thanks
rags

Follow Aerodark's advice and use that end mill... and carefully.

Drill 'drag' is not your only issue. I own a now banana-shaped Silver&Deming knock-off 3/4" drill that survived just ONE attempt to open-up a nominally 5/8" as-cast hole in a 1942 Monarch's base casting.

Castings can be irregular. May have inclusions and or variations in surface and near-surface hardness. And WILL have draft-angles.

(I say 'knock off' 'coz a genuine S&D would probably have snapped before it bent...)

Bill

Use a short solid carbide drill and you won't have any problems. You will be amazed by the stiffness of these tools. We routinely drill about that size into a face that is angled at 45 degrees. It makes a little noise, but location and diameter are good and the tools last forever.

Plunge an end mill that size. If additional depth is required, follow with same size drill

2nd this

although a carbide drill will probably work, an end mill (evan HSS)should survive casting irregularities and inclusions better than a drill
and if you need to face off a bos your already at the detail!
Mike

Originally Posted by ewlsey

Use a short solid carbide drill and you won't have any problems. You will be amazed by the stiffness of these tools. We routinely drill about that size into a face that is angled at 45 degrees. It makes a little noise, but location and diameter are good and the tools last forever.

Aluminium being far less likely to HAVE challenging inclusion crap as-cast, and softer as well vs cast iron, that may work, and work well.

But I'd sure rather bet on a HSS end-mill not breaking-off in the hole and leaving me with a 'blivet' than on a carbide - or any other - drill being as kind.

Regardless of material, drills are made for POINT cutting, not side. Flutes are ground to clear chips, and care taken that they do NOT also side-cut where not wanted, and multi-flute are not common. One flute at a time has to do the majority of the work, and in only a portion of its edge. Drills expect to support their tip's axis of rotation on the material in front of their cut, and it is only partially present when opening up an as-cast bore.

Plunge end-mills, conversely, do NOT expect such support, are ground for BOTH tip and side cutting, multi-flute are more common, so they are not only stiff under bending, they generate less concentrated bending force in the first place.

Bill

Core drills are made for that operation:

Core Drills, Fractional Sizes | Alvord-Polk

QB

thanks all,
your suggestions are most welcome, i have 3options

a. use an endmill - i think this is a bit slow

b use a carbide drill

c. use a slot drill - 2 flute centre cutting

i have had a few friends advising on a core drill - 3 flute core drill with a 30 deg relived chamfer nose.

any more suggestions.

thanks again
rags

Originally Posted by mjk

Plunge an end mill that size. If additional depth is required, follow with same size drill

2nd this

although a carbide drill will probably work, an end mill (evan HSS)should survive casting irregularities and inclusions better than a drill
and if you need to face off a bos your already at the detail!
Mike

Originally Posted by Question Boy

Core drills are made for that operation:

Core Drills, Fractional Sizes | Alvord-Polk

QB

As more commonly used the term 'core drill' refers to a drill which trepans, EG: Leaves a standing cylinder inside of its cut.

While those illustrated may indeed be intended for working with castings, I'd be suspicious as to a fit to the OP's need. More 'details' wanted, IOW.

Absent such, and catalog's as they are, they may simply have a draft angle so as to make core holes in PATTERNS that will release properly when cast.

Bill

Originally Posted by rags

i have had a few friends advising on a core drill - 3 flute core drill with a 30 deg relived chamfer nose.

That class of critter is sort of a cross between a drill and a longer-than-normal end mill. It should do fine in aluminium, so long the as-cast holes are straight, and you are not significantly off-existing-axis when opening them up. Downside is they are not as easy to find 'just anywhere'.

The common plunge end-mill, of course will happily move the hole if asked, and isn't overly worried about there even being one to follow. Mixed blessing, that.

Bill

Originally Posted by thermite

As more commonly used the term 'core drill' refers to a drill which trepans, EG: Leaves a standing cylinder inside of its cut.[...], they may simply have a draft angle so as to make core holes in PATTERNS that will release properly when cast.

I'm going to disagree about the "more commonly used" meaning of "core drill". Core drills are intended for enlarging cast cored holes, not for cutting tapered holes in patterns. They are typically three- or four-flute non-center-cutting. I've never seen a hollow one, much less one intentionally used for trepanning. Core drills are not a synomym for annular drill (aka rotabroach) or tapered end mill. Check out the KBC Tools catalog pages 34 and 35.

Core drills feed 50% or 100% faster than regular two-flute drills, but usually run at a reduced SFM. If you want them to improve location as well as size/taper of a cast hole, I'd strongly advise boring a short pilot hole before core drilling.

Originally Posted by sfriedberg

I'm going to disagree about the "more commonly used" meaning of "core drill".

The world is about more than just metalworking. Think concrete. Or just put the term 'core drill' (and not 'HSS core drill') into Google or call a rental agency .. then see how many of which type show up.

No disagreement on the patterns and draft-angle part.

My point was simply that the catalog page cited didn't specify even the 'basics' usually present on OTHER metalworking drills, as in 'n' degree, 'split-point', 'x' length, 'y' coated, 'z' finish, nor even WHICH HSS alloy from which they were made. Also uncharacteristically for drills as a class, that website doesn't seem to have the 'general' info further back up the 'breadcrumb' trail, either - I checked.

These pages DO have more of that sort of detail - some even as to recommended use:

HSS Drills, high speed steel drill , cobalt drills, carbide tipped drill, solid carbide drill , metric sizes , left hand, extra long , prentice, silver and deming, taper length

HSS Core Drill with Weldon Shank, 30 mm

Core Drills | Fastenal

I'm sure there are more to be found... Search term DID include 'HSS', so 'carbide' is another possible finder, though that one WILL pick up more concrete core drills than metal.

Bill

Cored holes off position are your biggest problem, any cutter not square across the cutting face will be guided by the hole to a greater or lesser exyent.

Short hole - I'd plunge with a 2 flute end mill - carbide if it's high silicon alu, over deep I'd still plunge with the end mill then follow up with a twist drill.

In AL it is as simple as throwing a Kennametal Tx drill at it. 5xd will have no problem going on size and on location with a relatively significant core shift. If core shift is usually good, you will get perfect holes. Are the parts die cast or sand cast?

Unless you have thousands of holes to make, I would just do a helical bore using a 1/4" or 5/16" 2-flute carbide endmill. You probably already have these in your tool inventory, and since the helix radius will be small, cycle times should be quick.

thanks a million guys, i will use all the options suggested and get back on the results
thanks again
rags

tried using an endmill, works ok , need to make more parts to check results
thanks again
rags