Looking for information on tool database settings for drills. I’m a new CNC hobbyist so I’m learning, but I am also a design engineer. I’m using Vcarve. What useful information I have found varies widely. My drills are number size stub length M42 carbide split point. Here are parameters that I have:
6000 Min RPM machine limit
Hole sizes from 1/4 down to .104 thru holes in 3/4 curly maple Janka 1450
SFM 300-400 for wood from a chart.
I have information that recommends speeds of 1500-3000 RPM that I would figure is meant for drill press. I have a chart that shows speeds for wood within the limits of the machine for the size ranges I am dealing with. I can make the calculations if I get some good advice from someone with some experience.
Anybody out there?
Congratulations on entering the CNC world! There is lots to learn about tools and the operations they can perform. Twist drills require much slower speeds than mills, and figuring out what works on your setup, in your particular material of choice, is a learning process.
You can bet that you’ll be breaking at least one drill in your CNC router as a result of learning.
In general, the smaller the tool diameter, the faster you can turn it. But remember, taking lots of little ‘bites’ on each revolution means that you cannot travel very fast (feed rate).
Most speeds and feeds charts are calculated for metal, meaning that they feed much more conservatively than what you would want for wood. They also have much higher rpm suggestions than what you want for wood. This makes sense when you consider how much more dense metals are than woods.
The moral of the story is that you want to turn far less than 6000 rpms for number drills, maybe more like in the hundreds of rpms. This takes router motors out the realm of possibility. A proper spindle is what you will need. Do you have a spindle or a router motor?
You can use twist bits on the CNC router, with some caveats. You have to get your router running a bit slower. I have over ridden the min speed on min so I can run down to 500 rpm. If you run at 6k rpm, especially on bits >0.25" you will likely burn the holes. I am told the newer frequency drive that comes with the new Hiteco spindles won’t go down to lower speeds, but I can’t verify that. If you can get it down to 2k, you will probably be ok for most small bits. You have to take it easy with long thin twist bits because they want to deflect when starting (you can always start them with an endmil and come back and drill). Using peck drilling to keep the chips cleaned out is a must as well. Here is a video I did last year on the topic. Drilling with standard twist bits on an AVID CNC Router - YouTube
jim
I have had no issues drilling in hard maple from 1/16 - 3/16 using 6000 RPM, 100” peck depth and .125” retract to clear the chips. I use to program a full retraction after each peck but found it wasn’t necessary. Depth up to 4xDiameter with no burning. 1/4” I use an endmill to plung and interpolate anything larger. Speed burns, but Jim is right, keeping the flutes from packing with chips makes a world of diffence. Don’t pamper the bit on the feed, IMHO. If you do, your burnishing and dust burns much faster than an actual chip. I can confirm the Hiteco will not run below 6,000 RPM.
You might want to check out stub length drill bits. You can get them in sets or individual. They are shorter length bits. I use these to drill holes from time to time. You just need a collet size to exactly match whatever drill bit you are using.
My thinking was you’d be less likely to bend a shorter bit VS a longer one.
Rule of thumb is that you need a higher drilling RPM the smaller the bit. There are a fair amount of charts and information you can find.
If you get a bit or a bit set from a quality retailer they might have this information for you.
Jobber bits are the standard length. What you are talking about are stub drills. I already have an M42 # set. They can handle 30% more RPM than HSS. Being that 6000 RPM min spindle speed already way exceeds the standard speed rating for the bits, I shouldn’t have to increase it for any size bit.
For the speeds I used to loosely follow guides for machinists like this one:
This was of course back when I had a self feeding air drill on my machine. That ran between 2k and 3k RPM. The spindle could run faster. When I was doing plastic production and I had to use tiny bits I would run them in the spindle to hit the RPM I needed, for bigger bits that needed slower RPM I would relegate those to the air drill.
I was mostly doing HDPE, acrylic and polycarbonate that way and things seemed to work well.
I’m no expert but that all seemed to work well for me. I got very long life out of my drills.