Tooling for Shaping Solid Wood Panel Edges on the CNC

A CNC owner gets advice on tool selection and CNC operation for profiling the curved edges of a 2.5-inch-thick solid wood countertop.March 13, 2014

I have a project that involves a few 9' long 2-1/4" thick maple countertops with all curved edges. The construction will be resawn hard maple veneer with solid maple edges. Material is hard maple with Baltic birch core. The edges of the counters will be a bevel on the underside but sort of an elliptical curve shape. Anyhow, these slabs are way too big to even consider profiling the edges on the shaper, so I'm going to do it on the CNC by padding up the slabs and having knives made for the edge profile. My question is about the tooling. I could have a custom 2-wing CNC router bit made for about $350 to do the edge. I have an ISO-30 spindle. Alternatively, I am considering using loose 5/16" thick corrugated knives and putting a standard corrugated knife shaper head on the spindle by using one of the ISO-30 1-1/4" arbors available from Vortex or Schmidt.

Does anyone have experience running corrugated HSS knives on the CNC? Other than wearing my flak jacket and standing behind a concrete barrier during operation, any other advice on the custom bit versus the HSS loose knives? I'm leaning strongly towards the loose knives since it will open up a whole new capability of running any of my shaper profiles on my CNC. I can run my CNC spindle in reverse, so all my shaper knives will work up to a certain height. I don't expect to ever need to run a profile taller than about 2 to 2.5".

I know that I need to take it easy when turning that much steel on the CNC. The overall depth of the profile is an inch or slightly more, so I would do multiple passes only taking off a small amount (1/16 maybe?) per pass.

Forum Responses
(CNC Forum)
From contributor B:
I doubt you need to be told but give serious consideration to RPM of the cutter head.

From the original questioner:
I was assuming to run it no faster than I'd run on my shaper. I'd usually run something like this at about 6000-7000 rpm. I'm not sure if there's an argument to run faster or slower on the CNC compared to the shaper. I'm going to take off a lot less than I would on the shaper since the shaper spindle is very rigidly fixed to a good 1500 lbs of steel, while this spindle is moving.

From contributor Z:

We do this all of the time on our 5 axis router to cut curved moldings and handrail parts. You just need to make sure the knives and gibs are balanced well. And set your rpm to the minimum to get full torque. Our spindle doesn't reach full torque until 9000 rpm. So that is the spindle speed we use when cutting with moulder knives. If you don't have full torque you can cause premature spindle wear.

From the original questioner:
Nice machine. I know a guy with a 5 axis Routech and have seen the machine in action. Very sweet. I will contact HSD about the torque vs. rpm question. Very good point.

Do you know at what RPM you run your corrugated head? My HSD spindle seems to not reach full torque until 12,000 rpm. Way too fast. I'll call HSD and see what they think about this. It's not like I'm going to be doing this a lot and I would be content to take very light passes to minimize strain on the spindle. Thanks for your input.

From contributor B:
Would you mind posting what HSD tells you?

From the original questioner:
HSD says that a "very heavy cut," which I interpreted to mean one that would threaten to shorten the life of your spindle, would be one that demands a 25% increase in current compared to spinning in free air (but with the tool in the spindle). He recommended that I take passes that result in a current draw increase of 10% above free air current, not higher. This was somewhat surprising. I would have expected higher percentages.

He also pointed out that full torque occurs at >12,000 rpm, at which point the spindle is developing 2 Newton-meters torque, but at around 7000 rpm I might be at 1.7 or 1.8NM. Come to think of it, it's not clear to me now whether the 10% and 25% recommendations were at the reduced torque or full torque. I'll have to find out.

He suspected that passes taking off 1/32 or 1/16 would be within range but could not say for certain (not surprisingly). I would have to experiment with feed speed and depth of cut and see what my current draw becomes.

Alternatively I could just have a custom router bit made, run at higher rpm, higher torque, and perhaps protect the spindle.

From contributor M:
At my previous employer we had a tool holder designed to use the same knives used in the 4 head moulder. This was an off the shelf tool holder, not a custom made one. Yes we did have to slow down the RPM,s but it varied depending on what the final diameter of the tool ended up being with the knives installed. Also somewhat on the bite that the knives made.

From contributor Z:
We run corrugated back knives on our CNC at 9000 rpm in a 4" dia head just like we may use on a shaper. The head has been dynamically balanced to 12000 rpm and then we balance the gibs and knives as a pair to .1 gram. I have run at 12000 rpm on highly figured woods and it runs smooth as silk. I routinely make cuts at full depth of the profile, whatever that may be. Since you are at full torque you can do this. I understand that it seems fast, but if the tool is balanced, the weight is not as significant. We use a HSK 100mm long stub spindle to run these heads. It is very versatile, and allows us to use all of our moulder profiles on the CNC.

From the original questioner:
Thanks. Points taken on rpm and balance. I forgot to add that I'm running a far more modest CNC compared to your Routech. Mine is a FMT 5'x10' 3-axis machine with the HSD 5hp spindle. A baby compared to that monster 5-axis. You also have a big enclosure around your spindle, while I do not. I'll definitely be behind a shield of some sort when it's running.

I should think the 5hp is plenty for what I need to do in any case. My smaller shaper is a 5 horse and I've never bogged it down. Frankly I've never quite understood why big CNCs have so much HP... typically they're removing much less wood than a shaper, and few shapers go above 7.5hp, maybe 10hp at the very most.

From contributor I:
Any cutting tool should not exceed 15,000 SFM and this is strictly a function of RPM and tool diameter. When you get above that number, steel can and does just simply come apart. To calculate SFM, you multiply PI x diameter x RPM and divide by 12 = SFM.

I would suggest you buy a dedicated tool (from a safety standpoint) but if you do decide to run the loose knives, I would stick to somewhere between 10k and 12k on the SFM.

From the original questioner:
So if I follow you correctly, SFM (S stands for what?) would seem to be the linear speed of the cutting edge?

(pi) * (5" cutting circle) * (12000rpm to get full torque) / (12) = 15,707 SFM.

Shrapnel time. Too fast. So to keep in your range, let's say a target of 11,000 SFM, I should max out RPM at about 8400 for the 5" cutting circle. Sound correct?

From contributor G:
Nice piece of kit, contributor Z. I have a 5 axis myself and it always surprises you what you can do with them. Have you ever crashed it?

From the original questioner:
I talked to Dimensions-In-Tooling today (maker of very nice custom tooling, if anybody is in the market for it). They made my insert carbide cope and stick heads and they're very sweet. It seems they may have a good solution. They can make an aluminum head for 5/16 corrugated HSS knives that greatly reduces the cutting circle compared to a standard 4" diameter steel shaper head. They balance it to 12,000 rpm (which includes a 2.0 safety margin for knives balanced to within 2.5 grams of each other... I will have to get a scale to weigh my knife pairs before loading).

The knives are not installed radially like they are on a shaper head, but more like a Hussey head, giving a cut circle diameter of close to 3", allowing for higher RPM and therefore greater torque and safety at a given RPM. I'm waiting for an engineering drawing, but it sounds like a good solution. I don't think I'd run it at 12,000, but 9000 or 10,000 would be nice. I would get an ISO-30 arbor and they suggest counter-boring the bottom of the head to recess the arbor nut, allowing the knife to reach the surface of the spoilboard if necessary.

From contributor Z:
This is your best bet. Get the higher rpm and still use HSS. I have some heads with a counterbore in the bottom and they are great.