Boring Block Bit Set-Up
Advice on setting up a CNC drill bank for good boring performance. October 12, 2007
I have a 20 bits drill bank. There are 10 in the x-axis, 9 in the y-axis, and 1 shared by both axes. I mainly want to use this machine to do 32mm line drill throughs, using 5mm B-point bits, from top to bottom of a panel. I also need to sometimes use an 8mm, 10mm, 20mm, and 35mm brad point. How should I load the drilling head? I sometimes need to drill halfway through a panel. Should I use the V-point bits for that or should I dedicate brad point bits for that?
From contributor K:
It depends on the kind of machine. Is it a nested base machine or pod and rail?
From contributor S:
You don't want to drill through with a brad-point, as you'll blow out the back side. I would dedicate the X for 5mm (all10), and throw the other diameters in Y. Use the bradpoint for "half-way through." If you are primarily drilling through, just change to b-point when required, or load 8 V and 2 B-point. Keep your pods out of the way for through-boring.
From contributor R:
Ditto with contributor S. Our normal setup has 2 brad points on the outside of the x axis. Keep in mind the mirror image if your machine runs that way. If we have a large run with brad points, then we switch them all out in the x axis.
From contributor M:
The location of the tooling in your drill block is very important. This will determine how many times the drill head must move in Z axis to bore holes, and it also determines how fast each cycle will take. This is not always a simple task. You may want to get a stopwatch and keep playing with the locations until your cycle time is right. It took me many months to determine the best setup when we purchased our first P2P many years ago. I kept switching the bits around until I found a good cycle time. You may not have enough pressure running a 35mm hinge bit in the drill bank. You might need to run this in a router spindle. You might find out the 35mm won't drill to full depth in drill block. You need to make sure that any bits with large diameters are kept sharp so that they don't have to have a lot of pressure to drill properly.
From contributor I:
Is the machine program based on tool number only or can you also program based on hole diameter? If it's hole diameter, then put the oddball tools at the outer ends of the drill bank (away from the shared spindle). This should allow the greatest flexibility for your needs. I also agree that you do not want to use brad points to drill through a part unless you drill halfway through from both sides. As for contributor M's comments about the 35mm bit, slow down the feed rate and set a slightly longer dwell time at the bottom of the stroke. It should work just fine then.
From the original questioner:
Thanks everyone! I will be putting 8 V-points and 3 brads in the x-axis, and the other bits in the Y-axis. And yes, I can program by tool or diameter. I will be using the dwell time feature for the 35mm bit, as otherwise the tool does not perform well.
From contributor I:
Okay... If you program by diameter, then I will throw out one more suggestion to streamline your process. The first thing is to decide which drill to lie to the machine about (either brad point or through point). The reason for lying is because the machine may not know the difference between the two. The way around it is to program one type as either 4.8mm or 5.2 mm and set the internal tool parameters to match this size. The other type is then entered as a true 5mm (or whatever size you want to do this with). Then you can always be sure that the proper one will come down for the given operation. If you don't do this, you may have the lance of a through point poking through the back of your part, or you might have a huge blowout on the back of your part when the wrong tool comes down.