cutting through 1 inch hardwood

[dave_k]

I'm not a newbie but want to do something I have never done yet, cut a swan shaped cutting board from a 1 inch thick hardwood blank. I have the toolpath, with tabs, but before I start breaking $50 bits, I need a little advice... I'm assuming I will need to make many passes to get through the one inch... maybe 4 or 5? This will be oak, cherry and walnut... so should I use a 1/4 spiral or a 3/8 with more beef? How deep a cut and at what speed can I get away with before I snap a bit in two?

I'm running a BT32 Alpha with a router

[bleeth]

How aggresive you cut will have some to do with the bit geometry but you should be quite safe at stepdown = diameter.
Some hardwoods are harder than others! Assuming this is white maple the above should work fine.

[dave_k]

Thanks Dave, I now have a ballpark to start with. Been searching other posts trying to glean info on this. found somebody doing 1/4 inch step downs with 1/4 inch down spiral at 2 ips which confirms your advice, but gosh I thought that was a bit too fast (no pun intended). I know from cutting osage orange and also black locust, that some hardwoods are harder and tougher to get through than cherry or walnut. Like everything else I do on this bot... I need to start conservatively and then up the ante little bit at a time till it starts looking hairy. Trial and error. Just hate when I ruin a bit doing that.

[blackhawk]

I have cut 1-1/2" thick hard maple for cutting boards. I use a 3/8" downcut spiral form Centurion. .25" deep passes, 2 IPS, 19000 rpm with a router. You would be fine with a 1/4" endmill also, maybe just back the depth of cut down to 3/16" per pass. You'll be able to tell if the router is straining or not, but these are good starting points.

[Xray]

I'd go with an endmill, jack up the speed [20,000rpm+] and slow down the feed rate 50-75%. I've cut 1" Brazilian cherry like that no problem, and that is some of the hardest, densest wood I have ever seen.
Probably know this, but if you use a spiral and it is tapered, you can expect a beveled edge.

[knight_toolworks]

I cut a lot of solid wood. I don't usually push it. 1ips 8k rpm and 1/4" and up you can do 1/2" per pass. I go faster when pocketing solid wood. but this speed has never broke a bit and keeps the vibration down somewhat. I cut a lot of purpleheart and ipe and these speeds always work. I always use a downcut bit to keep it clean and keep the parts in place.Now when your cutting 3" deep then you have to go to a 1/2" bit

[mzettl]

I make cutting boards from 2" thick Brazilian cherry using a 3/8" down spiral from Centurion at 1"/sec, 10-12,000 RPM, and 1/2" stepdown, very similar to what Steve does. I cut hardwood almost exclusively. I would respectfully disagree with the recommendation to increase the RPM and decrease the feed rate. This may cause the bit to overheat, causing premature dulling and increasing the risk of breakage. Feel the bit after you are done cutting. If it is too hot to touch, then either your feed rate is too low, or the RPM too high, or a combination of both. I have never broken a 3/8" bit. The problem for me is holding the workpiece securely if I increase the feed rate or the depth of cut too much.

Matt

[GlenP]

Your speeds and depths will depend on your bit quality and sharpness as well as material density or hardness. I cut allot of solid wood as well. I cut down 1/4" at a time and usually at 2-3 ips but will slow things down if bit is making unusual noises. That is something I find helpful is to listen to your bit while cutting. You will get so you can determine if something is not right by sounds coming from cutter.
One other thing I do to try and reduce cleanup (sanding) after cutting is to cut down around 80-90% of the way with a slight offset outwards (1/32") and then do a final pass cutting all the way through the material with no offset. It eliminates any step down lines that you may get from cutting down 1/4" with each pass to final depth. :)

[kartracer63]

I like that idea Glen. I've had those step down lines in some maple cribbage boards I've cut out. Seems like your idea might save some sanding time.

[harryball]

Without agreeing or disagreeing I will chime in with my formula and experience. Use at your own risk.

With solid hardwoods I start with 1ips and pass depths = bit diameter with a chip load of .01 (unless I have an odd bit or a bit with chip load data)

I always *try* to use a 1/4" up spiral bit for cutting operations (make sure it is sharp/newish). Ive found 3/8" and 1/2" bits seem to have more pushing force. I will use a straight or down spiral if hold down is an issue or excessive tear out.

After a few test cuts I'll make my adjustments. While "beta" cutting I use an infrared thermometer to check the bit temp, too high and I increase the chip load. I look at the physical chips to make sure they look "right". If you are not sure what right is, take a peice of the wood and run it through your table saw at a moderate speed on a sharp blade. You don't get dust, you get chips.

In production you'll get a feel for it and keep adjusting. You may find increasing RPM and cut speed to 2ips works great, go for it. You have to realize there are two mindsets at work on this forum. Some keep slowing down and others keep speeding up. I am the latter. I always think I'm running the RPM's and cut speed too low. I will likely break bits (and have) before starting a fire. Other guys keep slowing down, if not careful they end up with dust and bits that dull quickly from the excessive heat. Either way, the bit is dead.

From there, just keep it safe.

/RB

[dlcw]

The thing to remember when cutting any wood on the CNC is:

A screaming bit is a hungry bit.

If your bit is screaming you are feeding to slow or the spindle is running to fast.

I use a 1/4" down spiral bit (reduces kerf waste) cutting at 1/4" pass depth. Thickness of wood does not change my cutting strategy.

- For solid quarter sawn white oak or hickory I set at 3-4ips with spindle RPM at 9K - 10K.

- For bubinga I cut at 2-3ips with spindle RPM at 10K-11K.

- For hard maple I set at 2-3ips with spindle RPM at 9K-10K.

- For alder, cherry or walnut I cut at 3-4ips with spindle RPM at 8K-9K.

I make the majority of the cut in a climb direction (pushes bit away from the cut line) about 1/64" from the final cut line and leave a 1/32" skin. Then make a final conventional pass (on the cut line) to clean up the cut eliminating step down marks and making for a really clean cut. I've found this process is needed considering the amount of inherent flex in the ShopBot machines.

[Joe Porter]

I'M sure you already know this, but I always ramp my cuts using the spiral down setting. joe

[knight_toolworks]

I have been thinking of cutting less deep per pass and faster. should keep the heat down. Now I just need to remember to do it.

[dave_k]

Thanks guys... I've been away from the computer for few days. Great to come back and see some good ideas and logic behind them re: cutting my thick hardwood stock I plan on doing. One of the reasons I went with a ShopBot was all the great support they have in this forum. Nobody ever has to reinvent the wheel. That saves time, and THAT saves money. I have some great ballpark figures to start with from several of you that have been doing this, thanks again. OK, if the bit is hot or screams at me, I'm feeding too slow or spinning too fast. I like dlcw's idea of most of the cut being climb, so it's not digging TOWARDS the cut line, and also like the idea several guys had of doing my step downs with an offset, then a final 1/32 clean-up pass right on the line to eliminate some sanding. I already sort of use that idea when hogging out a cracker holder I sell a lot of (basically a 12 inch long, 1 inch deep "tray" that holds a row of saltines). I hog out the thing with a 1 inch strait bit plunging it every 3/4 inch, then clean out the tray sides and bottom to exact dimensions in five passes with a 1/2 inch solid carbide downspiral.

[michael_schwartz]

I primarily cut hardwoods.

I usually cut at either .25 - .5 deep at about 1.5-3 IPS. I have a PC router so I set the speed somewhat higher than what would be considered ideal to make up for the RPM loss. One of these days I will upgrade to a spindle......

When accuracy is of concern I create a profile tool path set to a climb cut and set the allowance offset to around .005-.01 I then copy this tool path to preserve tabs and other settings, set the allowance to 0, with a conventional cut. I often set the "finishing" pass to cut full depth.

[majohnson]

On cutting hardwoods, I use two different approaches, on wood like maple that don't chip easily I run 3/16" downcut at 1.5 ips. On chip prone woods, it goes down .7 to .9 ips. As far as depth, I use 50% of the cutter diameter. I'm running a PC router, at higher speeds 14k and up. I don't see pushing big bits, because of the waste factor, heat, and general wear and tear on equipment. I use a lot of exotic woods, some aren't cutter friendly so pushing thing to fast just becomes an expensive mistake.