Your advice PLEASE - surfacing bits

Hello folks!
I’m stuck and I’m hoping some of you knowledgeable people can help me out. I have an AVID Pro 60x120 with the Hiteco 3.7 KW spindle. I don’t have a planer or jointer in my shop so when I need to I use the machine for this. It works great. The planing is a little slow using a 1/2 bit so I’ve been trying to get some bigger surfacing bits to work for this.

Ive tried the really big 2" Whiteside 6220 and the somewhat smaller 1-1/8" Amana 45525. In both cases I started with the recommended feed/speeds in the tool databases that Whiteside and Amana provide for these bits. They work but they they burn the surface and overheat the bits. For both bits I have tried edging down the spindle speed hoping that a sweet spot could be found with no luck. In fact, when I got the 6220 bit down to 9200 RPM the spindle stalled - It was sitll burning the material.

I’ve tried this with white oak, maple, and baltic birch plywood with the same result. Are these bits just wrong for hardwood? or is it that my spindle doesn’t have the power required to use these bits at the right speed? Or am I just missing something important about how to set up cuts using these bits? I’d love to hear your thoughts!

What were the recommended feeds and speeds that you started with?

9200, as you found it is far too slow.

I can probably weigh in more when you tell me what speeds you started off at, but to avoid burning bits it’s all about chip evacuation. With those big fly cutter type of bits I see people start off too slow and they burn them almost immediately.

When I first started using those I started out “light and fast”. As in I took a light bite (something like .0625 per pass) at around 16k RPM at 200-300 IPM. (I was planing down a hard maple slab)

I keep increasing the bite, but keeping the RPM and feedrate the same. I don’t recall exactly but I think I settled on about .125 per pass. I’d call that a conservative cut that doesn’t destroy bits.

Here’s a comparison with the 3HP and our 8.7HP spindle, you can see more aggressive feeds and speeds here:

Our friends over at Canadian Woodworks do a lot of slabbing too:

Hi Eric!
Thanks for the insight. Here are the settings I started with:
6225 - 15K RPM, 200IPM, pass depth .050"
45525 - 18K RPM, 110 IPM, pass depth .125"
But with the 45525 the cut depth was less than the 1/8" pass depth because I was taking off much less depth (like 50 thou)

Slab slayer from RIP precision tools

Hi Eric,
Are you suggesting to cut deeper rather than slowing down the spindle or speeding up the feed?

I use this and it works GREAT!
Amana Tool RC-2263

1 Like

I 've been using a 6220 successfully on MDF (haven’t tested hardwood) without any burning setting the parameters to the following values. The tool diameter, of course, should be set at 2 inches:

Pass depth: .02 inches
Stepover: 1.75 inches (87.5%)
Spindle Speed: 15000 RPM
Feed Rate: 200 inches/min
Plunge Rate: 20 inches/min

By the way, make sure you have leveled the table and trammed the spindle carefully before surfacing.

Second 3 wing cutters with just the tips pointing down ie Amana 2263 but maybe a bit smaller 2255 or 2267. I use 2267 at 18K 200ipm 40th ie 1mm doc (double that doc for flatten way out of wack board that’s to big for 16” joiner) on all kinds or stuff from MDF to rock maple. Ya I take light passes. If you buy a bit with those sort of flat or parallel to surface slicers a lot of folks have had burning and just remove the slicer inserts. Note there are different carbide inserts available for different materials I have hardwood and MDF but usually forget to switch them out.

I think you’re cutting a little too conservatively here. Chips of wood carry away heat. Heat is the enemy of bits.

It’s a little hard to say “this is the right answer” because every piece of wood/bit is different, but what I’m seeing is that you’re cutting too slow and taking off too little material.

I’d say 15k RPM, 200 IPM and .125 per pass is a minimum starting point. Those settings should be good unless you’re cutting something crazy hard like IPE. From there I’d push it more it things are going well. Bump up the speed, RPM and cut depth. Do it in increments.

Just remember, you have a 4HP spindle and that 3HP in the video above was going WAY harder than what you’re doing now.

1 Like

I run the slab slayer, best surfacing bit in my opinion. I have run a lot of different ones and feel comfortable recommending the slab slayer.

Ditto. Why is there a 20 character limit on a response? Annoying.

Thanks for all the tips guys. Erik I’ll take your advice when I get back at it and start it at 15000/200IPM/.125" and speed up from there in increments if neeeded. Wish me luck! :sweat_smile:

Okay I tried it. the 6225
15000 RPM/200IPM/.125 depth.
The spindle stalled (the bit dug in about 50 thou and stopped ) and it jammed the machine. Maybe my Ramp in setting is too short? I haven’t used a tool that needs a ramp in but I think this one surely does. I chose 2".

Hi again Eric,
I tried it again with a 20" ramp so I could be positive that the tool wasn’t bottoming out. It ramped in to a depth of about .1" before the spindle stalled.

I get what you are saying about the 4 Hp in my spindle and to be honest I just don’t know if a 4 HP spindle is supposed to be able to do this. If it is, maybe my spindle isn’t delivering full power for some reason. Do you think that stalling the spindle like that is damaging it? It seems like Mach4 is turning it off. The spindle turns off but the tool path keeps going, causing the steppers to miss steps. It’s quite a spectacle actually!

One suggestion when planning. Make the pattern larger than the peice by atleast the diameter of the bit. This way no plunging cuts on top of the peice so its cleaner and no burning from the cutter stopping and changing directions. Say your peice is 12x24, with a 2 inch cutter make the pattern 16x28 minimum. Set the ramp to 0 and then no vertical cutting only lateral.


Not sure what kind of wood you’re cutting, but I’d drop the speed and see what that gets you. One thing you have to be aware of with hardwood is that you can hit a knot or a more dense section.

Just for reference, with my Amana Tool RC-2263 I can cut hard mesquite at ~100ipm at 0.100" - 0.125". That is a 2-3/4" bit. This is with the 4hp spindle, and with the 3hp I had to back off the DOC and feedrate a little. The knots on mesquite are pretty hard so I have to reserve a little extra hp in case I hit one of those. I usually run at least 18k rpm. This kind of bit doesn’t burn much because it has a pretty small blade area on the very bottom of the cut.

That’s a nice looking bit. I’ll have to save up my allowance for it! Did you splurge for the 457-DLC “diamond-like carbon” blades for it or are you using the ones that come with it?

I’m just using the standard ones. Its good to have replacable blades, especially on mesquite. It has a lot of defects and bark and there is often dirt and grit in the cracks (besides the wood being very hard too). I’ve done a half dozen river tables and gone through a couple of the corners on the 4-way cutters.

1 Like