PDA

View Full Version : Need to make 20mm holes in MDF



IQChallenged
03-07-2012, 09:22 PM
I need to make a replacement table (spoilboard) for Festool multifunction table. It's made from 3/4" MDF with 20mm holes. I need some advice on specifically what kind of bit to use and any other advice on how to proceed. Thanks

txcncman
03-07-2012, 10:18 PM
Do you mean like this:

537.200.31 CMT Forstner Bit, 20 mm diameter, 8 mm shank - CMT Drill & Boring Bits - CMT Forstner Bits - Mike's Tools (http://www.mikestools.com/537-200-31-CMT-Forstner-Bit-20-mm-diameter-8-mm-shank.aspx)

IQChallenged
03-07-2012, 10:42 PM
Do you mean like this:

537.200.31 CMT Forstner Bit, 20 mm diameter, 8 mm shank - CMT Drill & Boring Bits - CMT Forstner Bits - Mike's Tools (http://www.mikestools.com/537-200-31-CMT-Forstner-Bit-20-mm-diameter-8-mm-shank.aspx)

Thanks. I should've mentioned that my spindle is a Bosch router, uses 1/4" and 1/2" shanks.

txcncman
03-07-2012, 10:55 PM
Are you CNCing it? Use a straight router bit and circular interpolation to size.

Get an 8 mm shank and press a bushing on it to 1/2" size.

IQChallenged
03-08-2012, 08:37 AM
Are you CNCing it? Use a straight router bit and circular interpolation to size.

Get an 8 mm shank and press a bushing on it to 1/2" size.

1. Do you know where I can get such a bushing?
2. By circular interpolation-- do you mean cutting the 20mm hole rather than a straight pecking routine?

Yes, I am going to CNC it.

ger21
03-08-2012, 10:09 AM
2. By circular interpolation-- do you mean cutting the 20mm hole rather than a straight pecking routine?

Yes, treat it as a 20mm pocketing operation.

I would not advise trying to fit that CMT forstner bit in a router. Even if you can get it to fit, the rpm will burn it up within a few holes.
You can get 20mm carbide tipped boring bits that have 10mm shanks, and will work at 5000 rpm, but, you still would need to drill fast, which takes a very strong and rigid machine, as even the carbide bits will dull quickly if the feedrate is too slow.

Routing them is most likely the best way to do it. I don't know how deep you need to go, but you can get 1/2" upcut spirals with about 2" cutting length. That's what I'd use.

IQChallenged
03-08-2012, 10:20 AM
Routing them is most likely the best way to do it. I don't know how deep you need to go, but you can get 1/2" upcut spirals with about 2" cutting length. That's what I'd use.

Not in one million years would I have thought that a gcode for a circle would be used rather than pecking with a 20mm tool. Shows the difference between a hobbyist and expert. Do you think Festool does it that way? Thanks

ger21
03-08-2012, 10:38 AM
No, they use a CNC with drilling spindles, and use the 20mm boring bits I mentioned. The CNC we have has 15 independant drilling spindles for boring bits. The one at my old job had 21 drilling spindles. These are $150,000 machines, though.

IQChallenged
03-08-2012, 11:15 AM
The one at my old job had 21 drilling spindles. These are $150,000 machines, though.

That must be why Festool gets about $150 per replacement board. Not a very big board, not all that many holes.

neilw20
03-09-2012, 09:07 AM
This is very verbose (or succinct if you think it is) to make it clear what the code is all about.


(Cut a 20mm hole with a 10mm cutter 5mm deep)
(make hole at X0,Y0)
G0 X0,Y0 (where you want the hole)
G0 Z1 ( as safe height)
M3 S4000 ( speed)
G0 X-5 (offset by the difference in radius [20-10]/2)
G3 I0 J0 Z-2 F100 (center is I,J like X,Y and a feedrate)
G3 I0 J0 Z-5 (keep going down and around)
G3 I0 J0 (last time around at final depth)
G0 X0 Y0 Z1 (back out of hole)
M5 (STOP)
M30 (all done)
You could simplify initial values by making it parametric but harder to read.
Depending on the material it may give a better finish with G2 (not climb milling)
Some material get a better finish when the cutter burnishes the surface. Acrylic for one.

IQChallenged
03-09-2012, 09:59 AM
This is very verbose to make it clear what the code is all about.


Thank you. I thought your post was very succinct.