Need advice on end mill

Discussion about Tooling and Fixtures. End Mills, Router Bits, Hold Downs, Fixtures, Etc.
Post Reply
Woodworker
Posts: 639
Joined: Tue Mar 11, 2014 1:37 am
Location: 5 miles north of Benson, NC

Need advice on end mill

Post by Woodworker » Thu Jul 24, 2014 12:55 pm

I have a project that will require 7mm & 8mm holes ~65mm deep. What would be the best way to do this and where would I find the correct mill?
BRuce - SO2 #4798 - IC's Z axis upgrade, customized Z rail and Z motor mount, spindle Dewalt 611

Auarhau
Posts: 243
Joined: Tue Feb 25, 2014 8:46 pm

Re: Need advice on end mill

Post by Auarhau » Thu Jul 24, 2014 1:11 pm

You don't mention what material you are using, and what the holes are for. Pretty much any standard flat end mill will do it. Just make a pocket that size. Or if you have a 8mm endmill (or normal drill bit if it's a through hole), then it's just peck drilling.
Or, sometimes I just use the cnc to mark out where I want the holes, then do them on the pillar drill.
ShapeOko 2. Nema 17 74 oz·in. GAUPS shield on Arduino Uno. DRV8825 Drivers x4 . Kress 1050 FME-1. Z Acme Screw. Threaded inserts table.

AlBorland
Posts: 75
Joined: Mon Jun 23, 2014 5:26 pm
Location: Austria

Re: Need advice on end mill

Post by AlBorland » Thu Jul 24, 2014 4:11 pm

65mm deep holes? I don't think you will find anything better than a spiral drill. If necessary, pre-drill with the Shapeoko and finish it on a drill press.

Even if you find an extra-long endmill to do a spiral descent, you could end up with a significantly smaller or bigger (depending on milling direction) hole on the other side due to bit deflection (and Shapeoko deflection ;) ). Depends on the stock material and the bit diameter.
Also make sure you can raise the collet of your spindle to >130mm (for safe travel over the stock), maybe you need to mount the spindle a bit higher.

Still think the drill press is your best bet, maybe you could also do it with the Shapeoko by drilling from both sides. I did that once for a 60mm deep slotted hole, where precision was not that critical.
Shapeoko2, 4xNEMA23, tinyg, Kress 1050, various Z axis modifications

WillAdams
Posts: 8604
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Need advice on end mill

Post by WillAdams » Thu Jul 24, 2014 4:49 pm

Another consideration is tooling expense, also machine time.

The proper tool for this is a drill press and a suitable drill bit --- go ahead and use the Shapeoko to drill a locating indent, but then take the workpiece to a drill press to make the actual hole. The drill bit will last longer than the end mill (and is more readily re-sharpened w/o changing its diameter) and should be less expensive and the hole will be more consistent and the press will make the hole much more quickly.
Shapeoko 3XL #0006 w/ Carbide Compact Router w/0.125″ and ¼″ Carbide 3D precision collets

WillAdams
Posts: 8604
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Need advice on end mill

Post by WillAdams » Thu Jul 24, 2014 4:52 pm

That said, if you're really anxious to do this w/ your machine, check out the Garr Tools bits I recommend here: http://www.shapeoko.com/wiki/index.php/ ... mendations

They changed their web site --- maybe this link will work: http://www.garrtool.com/;jsessionid=24B ... D5D08352EC

http://www.shapeoko.com/forum/viewtopic ... 834#p21601

I used mine to cut some Ipê recently, no huhu.
Shapeoko 3XL #0006 w/ Carbide Compact Router w/0.125″ and ¼″ Carbide 3D precision collets

criznach
Posts: 220
Joined: Sat Dec 14, 2013 5:28 pm
Location: Great Falls, Montana, USA

Re: Need advice on end mill

Post by criznach » Thu Jul 24, 2014 5:46 pm

Even if you are just making pilot holes to be finished with a drill press, I've found a few things that help make nice holes using the Shapeoko. I've tried drilling 1/8" holes with a drill bit and I had a lot of accuracy problems. Most of the problems were due to the gantry flexing when plunging. Or the bit walks on the material as it starts to grab. So now I use a smaller bit. For 6-7mm holes, I'd use a 3.175mm bit, and either do a profile or a pocket depending on the diameter, and whether it's a through-hole. For 3mm holes I've been using a 1.6mm 3 flute end mill. I try to always use a spiral lead-in in CamBam. This eliminates the fast plunge straight down. Also when you're using a spiral plunge, you can greatly reduce your depth per pass, because a pass is usually very fast - only 10-20mm of cutting. For example, for 3mm holes in aluminum, I used a 1.6mm bit, and an inside profile operation with a spiral lead-in. My depth of cut was .05mm per pass. Feed is 500mm/min. It takes a minute or so to drill a hole in 1/8" material, but they look great.

Woodworker
Posts: 639
Joined: Tue Mar 11, 2014 1:37 am
Location: 5 miles north of Benson, NC

Re: Need advice on end mill

Post by Woodworker » Thu Jul 24, 2014 5:57 pm

thanks for all the replies. the material is wood, several different species, and I have had inconsistent results with a drill press. seems on holes of that depth the bit deflects and the hole is not parallel to the block side. I was hoping to either mill the full sized hole or maybe just a pilot hole and finish on the drill press if necessary. I will look over the links provided and try several of the suggestions. Just drilling it on the SO2 I am guessing would not be any better than the drill press and i did not find a supplier of 7 or 8mm drill bits with a 1/4" shaft. ok, off to try and fin a mill long enough and then run some test once it arrives.
BRuce - SO2 #4798 - IC's Z axis upgrade, customized Z rail and Z motor mount, spindle Dewalt 611

DanMc
Posts: 257
Joined: Fri Apr 13, 2012 3:34 am

Re: Need advice on end mill

Post by DanMc » Fri Jul 25, 2014 1:05 am

I've tried drilling using regular bits in place of an end mill and it did not go well. Most drills are meant for much slower rpm than the spindles we are using. I tried a couple 1/8" holes with my 300w spindle which was maxed out at 12k and it just snapped them, even at really slow feed and/or pecking. I can lower my rpms but haven't tried as end mills give a pretty nice hole, but a router or cutoff tool at 20k I think is too much for a drill meant to spin at 1500 or so. Just my 2 cents.

RobCee
Posts: 587
Joined: Wed Jan 08, 2014 11:33 am
Location: Birmingham, UK

Re: Need advice on end mill

Post by RobCee » Fri Jul 25, 2014 2:48 pm

For accurate drilling in wood, you are best to start small and work up to the size you actually need, usually in 2 or 3 stages. This gives best results with deep holes, but it takes time. The trick is to go slowly, as the grain can deflect the drill be quite a lot. Using stages allows the drill to stay on track better than doing it in one shot.
ShapeOko2 #3400 - Chinese 800W AC Spindle - Stiffened X-Axis - TR10 Z-Axis - Inverted Z Motor - Hall Effect Limits - Drag Chains & Custom Brackets

Nigel K Tolley
Posts: 226
Joined: Sat Feb 08, 2014 4:06 pm

Re: Need advice on end mill

Post by Nigel K Tolley » Sat Jul 26, 2014 1:02 pm

I'd recommend just buying a set of dedicated drillbits for wood.

However you could use a very short centering drill bit. Have the mill do a little dot in the right place, then use a drillbit to go through. If you want minimum deflection use a stubby drill bit first then a longer one.

I'm not sure if drilling with a smaller diameter bit first would help or not, but I find that in metals it just causes more bit vibration and wear, leading to a sort of triangular hole. So try it, but beware.

Post Reply