Boring Into Laminate on Plywood
Drilling into laminate-covered plywood poses a special challenge for a CNC router. Here are some tips on bit choice and machine settings. May 27, 2008
We are a countertop manufacturer fairly new to CNC. The task is to bore 3/4" deep, 10mm wide holes through laminate into 1" plywood. The question is which bit would be best, and never having used our boring spindles before, is it just as well to use a 10mm diameter tool to do the job with the main head? Machine is a Busellato Jet 3000.
From contributor M:
You can use a 10mm boring bit, but sometimes with laminate, there will be problems breaking through the plastic when using brad point bits. If the holes don't need a flat bottom, you will want to use a V-point (through bit) tool. If the brad point drill doesn't break through the laminate fast enough, it will be pushed back into the drill block as the machine moves in the z axis. This won't hurt the drill or the machine, but your hole may not be deep enough. I would not put a drill in the spindle. If you want to machine the hole with the spindle, use a smaller diameter bit and do a helical machining operation with an upshear bit. A downshear tool will create heat issues. A helical cut looks like a corkscrew from a 3D perspective. Use cutter compensation so you can control the size of the hole. If this is something you haven't done yet, refer to your programming manual.
From contributor V:
We do a bit of this with a normal drill bit (brad). I usually program the drop twice so if it doesn't go deep enough the first time, it will clear the hole on the second pass. Like contributor M says, the spindles are air operated, so can hold up on the first drop.
From contributor I:
What contributors M and D have failed to adequately explain is that when a brad point first cuts the laminate, the outer spurs will simply cut a small disk of laminate that then (if not firmly glued to the substrate) will spin on the substrate under the drill bit, thus preventing the drill from penetrating the substrate. You will encounter a lot of this since you are using a plywood substrate.
If you use contributor M's solution of routing holes, you have to slow your feed way down to prevent getting egg shaped holes. This will in turn heat up and subsequently dull your bit.
Contributor D's solution is closer. Drill it twice, but do the first hit with a smaller (8mm) through point bit and not to the full depth you need. Just enough to get the lance through the laminate. Then come back and hit it with the brad point bit at your final depth. This will prevent the laminate from causing problems.
From the original questioner:
Using two different tools isn't preferred, as we are doing many holes. 63 holes each in 87 boards as well as 20 smaller boards of 20 holes. Does that stir any new thoughts/techniques?
From contributor A:
Maybe you use a downshear router bit in a pocketing routine?
From contributor K:
Main head drills work great, but if you can drill multiple holes with the drill unit, that would be best. If you run into problems with the drill unit you should be able to insert a dwell or peck. If I knew Busellato I would tell you how, but I don't. If you don't know how, you should call tech support and they should tell you. Also you could turn the air pressure up at the drill unit, but it may slow retraction, which could cause problems. A carbide brad point should work fine.
From contributor B:
Use a v-point and drill as fast as possible without deflecting the part or overcoming the down force of the air cylinders on the drill spindle. Even your older Busellato uses two stacked air cylinders on each spindle for 63kg of down force. Program a 1/4 to 1/2 second dwell on each hole. The drill will pause at the bottom of the stroke for a few more revs to allow the material to relax if it is deflected to ensure accurate hole depth. Be sure to put pods as close as possible to the holes for good part support.
From contributor K:
If you need a hole 3/4" deep in a 1" panel you will poke through or damage the other side at 10mm diameter with a V-point or the hole won't really be 3/4" deep it will be closer to 1/2" deep. You can't count the 60 degree taper as part of the depth unless it doesn't matter.