I have been running 2 CNC routers for about 4 years now. I cut all the parts for my products on them and run them for thousands of hours. I can see that there is an interest in this technology and thought I might scatter some of my fairly random and very personal observations in this post in the hope that they might be useful to others .
This is massively important. My production system uses vacuum workholding. Each machine has its own vacuum pump and the workholding plates are made from phenolic ply and I use neoprene based tape for the seal. There are lots of ways of using vacuum - mine is pretty specific but if you are at all serious about using CNC invest some time and money to make a good solution for your own needs. For one offs where vacuuum isn't appropriate I generally make some drill holes in the workpiece away from the cutting lines and run a drilling program before the cutting program and screw through the workpiece into a spoilboard. There are other ways to hold workpieces but for any real volume some manner of vacuum system has to be the best solution
I've gone through several evolutions on this matter. Most of my work is profile cuts, in other words cuttting out the edge of a shaped workpiece.
I started out with 1/2" straight cutters. Disaster. Expensive, wasteful, noisy, limit the minimum internal radius of cuts. Not suitable for drilling pilot holes or cutting small holes. Disaster.
Then I tried 6mm spirals. Litttle bit less of a disaster. Expensive, wasteful. Tiny bit better for cutting small holes and slightly tighter radii.
I'm now on 1/8" (3.175mm spirals). Best solution so far. Cheap, relatively quieter. Perfect for drilling pilot holes and small radii. I have to make more passes at a shallower depth but for me the trade off is well worth it.
I'm cutting 3 identical components at the same time. If something goes phutt then I will usually lose three workpieces. I try hard to program for reliability. I would rather have 99.9% succcess in 10 minutes than 75% success in 5 minutes. Here are my rules for that.
1 - Don't speed. Things go wrong when you push the edge of the machines performance envelope. My machine will rapid (G0) at about 8M/min (call it 25 feet/min). But it will rapid alll day without a hiccough at 6M/min. For actual cuts I usually run rough cuts at 2.5M/min (8 feet-ish) and final cuts at 1.25M/min (4 feet-ish)
2 - Don't cut too deep. Most of my cuts are 23mm total. I typically take 5 passes of 4.6mm. Much deeper and I get too many broken bits. Much less and I'm wasting time. I nearly always program so that the component gets a rough cut to full depth in 5 passes but 0.1mm (work it out yourself) oversize. I then make one or more final passes at full deph without the oversize allowance. If I have the time I make 3 or 4 of these final passes which means that the commponent comes off with basically no need for any further edge finishing.
3 - Climb cut. All my cuts are made on the climb. I used to make the final cut "conventional" but I found that it resulted in frequent grain tearout or splittting along the grain which kills my vacuum and therefore the workpiece. Climb cuts are massively more reliable in the timbers I use with the cutters I use.
4 - Clear waste. Most of my SNAFU's came back to a loose waste offcut lying on the table snagging on the cutter head. All my programs now have a pause between the rough and final cuts so that I can safely remove loose waste. It only took me three years to work that out.
Sorry - got to run now - will try to pick this up with more thoughts tomorrow. If any of this doesn't make sense or if anyone has questions about running CNC let me know and I'll do my best