What options are there for mounting a drill bit and/or chuck into the machine? Is there a specification for a chuck that would fit where the ER-11 collet goes?
The Nomad is a bit limited in spindle torque nor does it support the drilling G codes. Could one drill with the Nomad if they are careful? Yes.
Is it possible to find a chuck that has a 1/4" shaft (so it fits the largest practical size for an ER11 collet)? Yes. The extra length of adding a chuck is going to severely restrict what you can do.
The ER11 collet is a standard. Take a look at collet vendors - MariTool is a good choice - and procure a set of ER11 collets that match the drill sizes appropriate for your needs.
mark
Thanks for the info. Is there any downside to milling a hole vs drilling it (assuming you are using a straight mill with no tapered neck)?
End mills are ~4 times better at going across than down. A drill is ~4 times better going down than across.
Yes, one can drill a hole with an end mill. Be sure to use a safe plunge rate and you’ll be fine.
MeshCAM uses a surface following process - it’s been discussed elsewhere - and puts a limit how small a hole MeshCAM can handle with an end mill.
The smallest hole that MeshCAM can deal with is ~10% bigger than the diameter of the end mill one specifies. MeshCAM will generate the necessary G code (machining instructions) to clear a hole.
The walls of the hole produced via an end mill are nice, but not as nice as those done with a drill. If you’ve got finish requirements for the holes, be sure to pencil finish them.
mark
P.S.
MeshCAM does handle true drilling. See:
http://www.grzsoftware.com/faq/drilling.html
The Nomad is where the limits come from, not MeshCAM.
One thing to note is that, while you can indeed put drill bits of the correct diameter into your spindle, you need to make sure they are the correct length (“screw machine” I think it’s called).
I stuck a regular (jobber) length bit into mine, and when it tried to measure it, the bit was so long it crashed at full rapids into the probe. Made a loud noise and could have been very very bad, but luckily I was watching it and hit the e-stop before any damage could occur.
Also, watching the nomad drill holes can be absolutely maddening. It pecks into a hole, moves to the next, pecks, moves, etc, then goes back to the first and does it again. Wildly inefficient! It’s worth it to try to work out how to make MeshCAM give you sensible drilling g-code. Or get it elsewhere…
And of course there are PC board drills, which are carbide and have standardized .125" shanks. I have bought drills and endmills from http://drillcity.stores.yahoo.net/ . They sell resharpened tools at a good price.
@MrHume, if you are seeing peck drilling,the gcode isn’t coming from MeshCAM. MC just does a single drilling move at each hole.
What you might be seeing is a spot drill move at each location followed by the actual drilling move at each location. By default, spot drilling is enabled, and also by default all the drill tool numbers are set at 1. Before you write the gcode you need to go into each enabled process and set separate tool numbers.
For the above job I disabled spotting and all but one of the hole sizes and generated the gcode, which came out as follows
%
(FILENAME: drill.nc)
(STOCK/BLOCK, 12.500, 5.150, 0.910, -0.000, -0.000, 0.910)
G20
G90
(TOOL/MILL,0.1100,0,1.0000,0.0)
M6 T1
M3 S5000
G0X0.0000Y0.0000Z0.5000
(Drilling)
G0X4.2154Y1.1563
G1A0.0000Z-0.9100F10.0
G0Z0.5000
G0X4.8846
G1Z-0.9100F10.0
G0Z0.5000
G0Y1.9437
G1Z-0.9100F10.0
G0Z0.5000
G0X4.2154
G1Z-0.9100F10.0
G0Z0.5000
G0Y3.9563
G1Z-0.9100F10.0
G0Z0.5000
G0X4.8846
G1Z-0.9100F10.0
G0Z0.5000
G0Y4.7437
G1Z-0.9100F10.0
G0Z0.5000
G0X4.2154
G1Z-0.9100F10.0
G0Z0.5000
G0X7.6154
G1Z-0.9100F10.0
G0Z0.5000
G0X8.2846
G1Z-0.9100F10.0
G0Z0.5000
G0Y3.9563
G1Z-0.9100F10.0
G0Z0.5000
G0X7.6154
G1Z-0.9100F10.0
G0Z0.5000
G0Y1.9437
G1Z-0.9100F10.0
G0Z0.5000
G0X8.2846
G1Z-0.9100F10.0
G0Z0.5000
G0Y1.1563
G1Z-0.9100F10.0
G0Z0.5000
G0X7.6154
G1Z-0.9100F10.0
G0Z0.5000
M5
M30
(END)
(OF PROGRAM)
Randy
For those new to drills, imperial drills were standardized a long time ago. If you haven’t been confused by a drill specification in a CAD drawing or WEB order page yet, you may be without the magic decoder ring. You have or will see things like a Q or a # 49.
A very long time ago, drill sizes were standardized. Small diameters are numbered, larger ones are lettered.
You can find complete tables online and local machine tool shops either give away or sell laminated cards that condense the information into a handy form. My machine tool box has such a card in the top.
Many WEB sites and catalogs are careful to list both the standard designator (letter or number) and the diameter.
mark
P.S.
Remember to ensure that your spoiler board is thick enough to handle a drill. If you’re drilling all the way through your stock, one must drill to the depth such that the head of the drill goes entirely through the stock - the shaft must clear the bottom of the stock.
These are my two “go-to” links for drill sizes. I have them right up on my Firefox bookmark bar. Easier to visit a page than look up a PDF on my hard drive every time…
http://www.engineersedge.com/drill_sizes.htm
http://www.newmantools.com/tapdrill.htm
Randy