Good morning, Happy New Year everyone!

I have owned my own CNC since around 2010, I have strictly cut cabinet parts with it, mainly all sheet goods, 3/4 inch max generally.

I want to do some solid work, mainly cutting 3/4 inch solid walnut and also building some tables so cutting 2 inch thick solid hardwood and also flattening the table top with a 2 inch diameter spoilboard type cutter.

I was wondering if the feed rates and depth of cuts are similar to the sheet goods I cut, I was also wondering about tooling’s
I have done a lot of reading and was thinking of using the same 3/8 compression bits I always use and multiple passes with the same feed rates as I do for sheet goods.

I just wanted to make sure I don’t have an iissue or cause an issue is maybe a better way to say it.

I will be using an SCM cnc with a large powered spindle.

I'd say the biggest challenge of cutting solid wood vs. panel stock is keeping the part solidly in place. Wood vibration while cutting can quickly lead to under sized parts and bit breakage.

There are a number of methods to hold the wood from screwing it down to secondary spoil board to vacuum pods. Examining the size and shapes of the parts you need to cut will determine what is going to work best for you.

I always found I could cut up to about 1" hard woods, held by vacuum pods, in one pass as long as the parts being cut were large enough, and shaped properly to be able to get multiple vac pods mounted in an arced pattern to do the job. Vac pods in a straight line (i.e. under a straight board) do not hold the wood solidly enough in place.

In the above situation I would cut at 18,000 rpm at about 200 ipm. I'd do three passes, the first a climb rough cut that would leave the part about 3/32" over wide due to part shift on the vac pod gaskets, the second in the same direction to bring the part down to final size, and the third a conventional cut to clean the edge.

BH Davis

Oh, I should add. 3/8" DS HSS bit.

Downcut spiral so the bit was pushing the wood down onto the vac pods instead of pulling up with an upcut spiral. HSS instead of carbide because the high RPM at the low feed rate, needed to help keep the wood on the pods, generates a lot of heat in the bit. HSS stands up to heat better than carbide. Also the HSS is less brittle than carbide so not quite so susceptible to breakage from the wood vibrating on the vac pods.

BH Davis

Lots of ways to skin this cat. Let me muddy the waters by sharing what works for me: If pods are a hassle like they are on my machine, and if the board won't hold down because it isn't milled dead flat or is too small in surface area, I use 3M 9832 double sided tape. It is seriously aggro and grips like nothing else I've used, and can tear chunks out of the spoilboard if not detached gently. If I'm cutting very small parts that fly away if cut loose, I leave a .040 skin when cutting the shapes out, then flip the board upside down and use more 3M tape to stick it down to some melamine and run the sandwich through the widebelt sander to sand off the skin and leave just the small parts attached to the melamine. It works really well. I've made crazy tiny parts this way.

Tooling depends on wood thickness. I personally can't stand the chatter that 1/4 and 3/8 bits emit when cutting solid wood, so I use a 1/2" 2 flute carbide for most applications. Upshear if the material is really locked down, otherwise downshear. If the wood is thicker than 1.5" I have a 3/4 dia chipbreaker that devours 3" thick maple. All tooling is carbide. If things go sideways, which is more likely with solid wood than plywood, I want the bit to shatter, not bend like I've experienced with HSS bits.

Feed & speeds: google a chip load chart like the one on Vortex's site. In theory you want to go as fast as possible before quality falls off, but in reality the priority hierarchy is: 1) the part must survive, and 2) avoid excess spindle wear by pushing your machine too fast. Premature cutter wear because you're cutting too slow. Depth of cut: definitely don't use the same cutting strategy as sheet goods. With the abovementioned 1/2" 2 flute, I would cut your 3/4 material with at least 2 steps.

A 1/2" carbide downcut spiral chipbreaker is my go-to bit for any solid wood parts I cut that are 3/4" thick or more. I can go up to 2.5" thick, cutting 1/2" each pass. For softer woods like alder, I use a feed rate of 300 ips. For harder stuff like oak, walnut and beech I feed at 200 ips. For round or oval table tops, half of your cut is against the grain and can be prone to tearout. If the final cut is not quite as clean as I'd like, I'll take about a 1/32" more off with a 1/2" compression spiral at full depth at get a smooth edge.

View higher quality, full size image (800 X 498)

A 3/8" diameter bit is going to be singing a tune, even when doing a final pass on 2" material. I never use a downcut, especially for doing step cutting in the roughing pass. A roughing bit is a must for me and then go to an uncut spiral for the finishing cut. Walnut is definitely not chippy, but a climb cut will help if you have some highly figured stock.

I would add if you can program end grain cuts separate from long grain you will be better off and stick w 1/2"dia or large down-spiral solid carbide w feeds and speeds listed above. The rational was first step through 1/8"per pass conventional CW cut on end grain and round over corners and let it blow out. Then blow n go with long grain climb cuts faster , & cut much deeper depending on vacuum / part holding strength. We did many of one-piece flow jigs for production work by band-sawing everything 1/8" oversize clamp into dedicated jig w Destego clamps mounted horizontal & route dowels / tenons in zone 1. Flip parts over into zone 2 onto mating locating tenons / dowels w dedicated vacuum bleed through for each part; route end grain 1st, and then long grain, for chair, barstool and table parts ready for pre-sand or assemble.

Mcmaster Carr has 3/8" & 5/16" nylon hex bolts & screw mount T nuts for alternate holding of parts if you don't have the numbers for a production type jig. Route in screw-in T nuts from btm of a dedicated 'parts' spoil board was another way to route onesies. In this scenario we would put tabs on end grain 'bolt islands' to hold the part and template route the part free after machining. " Allstar's Adhesive"CNC self adhesive 1/8"th rubber gasket was a goto for gripping the wood in any jig. This type of jig we would slow down the feeds and speeds and listen for sounds of vibration, but it worked.

The easiest way is to glue-up slabs and onion skin multiple part from one blank as mentioned above.

As said many ways . . . Best,
Tom

Im in the duster camp.

For me my answer with regards to your original question as to whether feeds and speed are the same is no way in the hot place.

There really is no uniform answer in my opinion especially when your getting into the 2" range even for a cleanup pass. Grain direction, as mentioned edge/long, how much tool engagement, and something I didnt see mentioned is machine rigidity. I'd say that, over spindle power, rules it all. If your machine isnt dead rigid your going to have to do a lot of working around. Chatter cut quality are a bear with solids especially when they are thick.

Like duster says, spirals are a good route. Compressions are a waste. Be careful with up spirals as they can act like a drill bit and rip your work off the table into the spindle. They are attractive for chip evacuation but a catch can be a spindle crushing day.

Avoid full tool engagement at all costs if you can (adaptive clearing if you have the ability. 2 pass clearing for deep stuff if you dont).

Surfacing is pretty straight forward. We surface with a 3.5" insert but realize that you will still need to leave a decent amount of material because you will have a LOT of sanding unless you single pass profile (no raster or offset clearing where tool runs back and forth). Even razor sharp tooling the slight tearout from opposing passes takes a lot to grind out.

I had a lot of trouble getting good finish on grainy woods like rift oak untill I started using a roughing bit .

If you cut first with a roughing bit and then clean up with a spiral or compression you can get great finish right off the router.

The roughing bit has a lot of wavy lines along the flute and really helps with tear out .

What is the percentage of the power of the spindle in the power demand of the entire machine tool? This needs to be analyzed and judged according to the power of the main power. Usually, the main power of the equipment is 70% of the entire machine tool.