5mm Holes in MDF

[Bob Eustace]

Never drilled holes with a 5mm dowel drill before (customer supplied) and I'm worried about the dirty big flat on the 10mm shank. Using an ER25 10mm collet. Using the small HSD spindle. Holes are 13mm deep. What speed should I use if this set up is OK? All advice greatly appreciated!

[jTr]

Bob,
Felt the same apprehension at first, but using same bit, same spindle, I have had complete success and experienced no problems. I cautiously started with a 9,000 rpm setting, and it works just fine. When punching 3/8 depth holes, all is well, though MDF does tend to get singed a little if you push 18mm (3/4") depth.
Set tool path utilizing hole drilling feature in partworks. Be sure to check "Peck" drilling which causes bit to be lifted out for chip clearing when you exceed 3/8" depth, which should help.

Good luck!
jeff

[Bob Eustace]

Thanks Jeff - guess I can skip the Valium!

[feinddj]

Bob,
Why even use a 5 mm bit? You can "drill" any sized hole you wish. I use a 5/32 bit to profile the inside of the hole on a ramped cut. Works like a charm.

David

[coryatjohn]

I would think the approach David mentioned would produce superior results.

[Simops]

Bob, I'm with David as well. I have used 1/8" upcut bits to cut holes down to 3.5mm using ramped profile.
I read on posts here before that it is not a good practice to drill holes with a spindle as the bearings in the spindle are not designed to take vertical forces.

Cheers

[bleeth]

I would imagine the drilling is for cabinet parts. Unless you have a seperate drill and/or twin routers/spindles I have found the whole process is easier to just use a 5mm bit from Centurian and do the boring, back dado, and part cutout all in one nest with no toolchange. Taking typical cabinet mix and my move speed (PRS Standard at 3ips) with that bit into account (3 pass cutout) I can cut about 9 full sheets in a day of cabinet sides with sheet change, labeling, and cleanup into account. While each sheet is cutting I cut tops, bottoms, nailers, stretchers and shelves on saw. Overall days production can be one heck of a pile of boxes ready for edgeband and assembly with no bit change.
I have had a longstanding discussion with someone who used his multibit tool to cut all parts on a much faster Alpha. If the boxes are being built for butt assembly it's a draw. He only wins when all parts must be cut on cnc due to blind mortise and tenon construction.
If your client is handing you cut parts and all you are doing is drilling, it sounds like an opportunity to upgrade his order.

BTW: I drill all shelf, drawers slide, and hinge holes with a peck strategy. Been doing it for years in a production shop with a 5HP Columbo. No problem. There are dedicated CNC controlled boring machines that uses spindles. HSD makes a multiherad boring attachment for their spindles. The bot about nopt boring is a disclaimer similar to don't eat 20 aspirin. As long as you use a proper strategy you should have no problem.

[dlcw]

I use 3mm, 1/8", 5mm, 1/4", 8mm, 3/8" and 1/2" boring bits on all kinds of material - MDF, melamine, plywood, solid. My standard feeds are 6500rpm @ 1ips. I drill in one plunge. I use the boring bits as pictured above. No chipping, no burning and perfect holes every time.

Still using the same bits I bought 3 years ago and they still drill perfectly.

Between spindle cooling fan and DC air movement, no heating of the bits. After drilling a couple hundred shelf pin holes in a sheet of melamine, the bit is room temperature when I go to change it.

[feinddj]

David here again,
One thing I forgot to mention was the ability to size the hole to a little wider or less than drawn by using the offset in the toolpath. It makes it very easy to size the hole to the pin by only changing one number.

D

[davidp]

Hi Bob,

From the photo it looks like a WD5R56 from Carbi-tool. They are used in hinge press machines. They are quite simply the very best tool to use to drill perfect holes. If you are drilling holes for shelf pins forget using a bit and cut the hole with a ramping path or even using a 5 mm end mill. Slow down your spindle and don't be too quick with the feed rate to allow the swarf to clear.

We drill hundreds of holes each month and have been using these bits for 8 years without a problem. In December we cut 40 sheets of 18mm ply that had over 2,400 holes per sheet in a very particular pattern and we used these bits. Perfect holes and quicker than any thing else.

There are two gotchas, one, as they are brad points, if drilling a through hole cut approx 2.5mm to 3 mm deeper to get past the point and the spur and, two, make sure that the drill is marked as an a R as they are also available in left twist. Other than that use them with confidence.

My grandfather used to say "why use a hammer to crack nuts when you have a nutcracker?". In other words if you have the correct tool at hand use it.

FWIW

David
Sydney

[Bob Eustace]

A million thanks for all the excellent advice - sincerely appreciated. This forum is just fantastic as I know most of you guys are super busy.

DAVE - Yes you are correct they are sides for bedside drawers in a hospice. As you have guessed we have very limited knowledge on this and dont normally touch this stuff as I hate repitition! On background the guy lost his shop and house in our horrific bushfires 3 years back. Sadly his customers all deserted him whilst he rebuilt. He eventually got a new guy doing this hospice stuff for but got swamped on the first order which is how we came to help out. He supplies us the stuff cut and edged. All the holes are doing is screwing on the runners. Now dont choke but we do this job as two ops (does your back in!!!!!) Now we already use Centurians 1/8 EMs but the these are only 1/2" cut depth (18DS2.52RES14) - we love his 1/4 compression bits!!!! Are you saying we should try to do this job with one set up???? Holes are 13mm deep and pockets 12mm. If so what speed/feed, DOC on the pockets?

[bleeth]

It could very well be that by the time you change bits and re zero the pockets would be cut by an area clear with the 5mm end mill using one bit, although you would be spending more time standing around watching so it could be a bit boring. (Sorry-couldn't resist the pun)
That seems a deep hole for a system screw. I drill mine around 7/16" when using the longer ones. Your pockets could be done safely with the 5mm in 2 passes and an 80-90 percent stepover.

[Bob Eustace]

Thanks everyone - got the job done with no hiccups (apart from comms on 3.8!) yes I do use ramped profile for holes all the time and learned easy on to us upcuts!

Don - used your speed and feed - worked great!

Dave - cant wait to give your suggestion a bash when time is not so constrained.

David - your post saved the day as I was very nervous about running a cutter with a dirty big flat on it! You might convert me to Carbitool yet!!