Routing Dimensional Lumber

Hello all I was running some tests today and I wanted to show you my findings as I hope it could help at least 1 person out

So what will we be routing today?

Pine, Lumber, Dimensional Lumber, Trash wood, Douglas Fir, white wood

there are many names for it but basically its the wood that you find at the home center in the form of 2x4, 2x6, 2x12, etc

Why do we want to CNC route this?

we because its cheap easily accessible and works for many things and if your really picky you can create knot free panels and projects

What tools are we going to use?

Support Tools

Jointer, Table saw, planer

We use these tools to square and prepare our stock in order to get it ready for milling.

CNC Tools

HSS (or carbide) Single Flute Downcut
Carbide 3-flute Low Helix Downcut Finisher

So lets start by thinking about what we are cutting

We are cutting soft wood and this means that things like tear-out and fuzzies will happen often and we are going to try and minimize that effect

Here is the material test we are going to run

this is a 6.5 wide x 8.75 long x 1" thick piece of pine. When testing materials its best to not skimp as you might make mistakes so give yourself room to explore many different CAM strategies

okay so basically we are going to make a pocket .75" deep with a couple circles and 1 circle with a pocket inside of it and run a test to test edge finishes please note that floor finishes are something we can tackle latter

this test really is only to test surface finish of 2d carving straight off the machine so there are no need for things like slots or complex shapes but we do want to be able to test the tools with the grain and across the grain

Here are the 2 tools that we are going to work with

1. 1/4" HSS (or carbide) Single Flute Downcut

I choose this tool because we are working in softwood and its paramount to maintain proper chipload and shearing action of the tool against the wood. Single Flute tools allow us to take a large chip per revolution out the the material while maintaining slower feedrates for smaller more flexible machines. Also single flute tools generally have a lower helix angle which is what we want when working in softwoods especially

Now I said HSS or Carbide personally I prefer HSS in this case even though I am a firm believer in everything Carbide. The theory is that HSS can hold a sharper edge than carbide because carbide is brittle and if you get it to thin then it will just chip and well I by that. So I went with a 1/4" HSS Downcut tool

I choose a down cut because I am just making a pocket here and I want a good top side finish and downcut tools will force the material towards the spoilboard providing better holding power

This tool will preform all out our roughing operations leaving .04" of stock to clean up later. This is VERY VERY you must leave stock to get a good finish even though you will get a decent finish with the single flute tool we can do better

Here are the settings I used for my test (your setting may vary but maintain the same chipload)
RPM: 22000
Feedrate: 132 ipm
Plunge Rate: 60 ipm
Lead-in/Lead-out Rate: 60 ipm
Chip Load: .006"
DOC: .25"
Stepover: .0825" 33% of tool diameter
Cutting Direction: Conventional

Remember your chipload formulas and always check your tooling manufactures chip load recommendations when programming to insure warranty and tool life if you cannot run at these setting then adjust accordingly to maintain chipload

2. 1/4" Carbide 3-Flute Down cut Low Helix Finisher please note the pic shows a upcut but we use a downcut here

I choose this tool because we want low helix flute geometry and we want to take small tall shavings off. Think of your 3-blade planer or jointer and how they make wood feel like glass when the blades are sharp.

Also a downcut spiral will provide better top finish, work-holding, and provide less chance of tear-out compared to straight bits

This tool will perform all the finishing operations and take that .04" of material off that we left in the roughing operation at FULL DEPTH

We want to run the tool at full depth to maximize the surface quality. Even though we are only running a small 1/4" tool we can go full depth in 1 pass because we are only taking off .04" radially. However it is just as important to use what they can Lead-in and Lead-out when finishing. This brings the tool down to depth away from the material and then pushes in and around the material at full depth. If you lower the spinning down straight down on the material you can leave behind a line caused by tool deflection. Ramping into the material can leave the same line

On your finishing pass you want to program into your toolpath at least .001" stock to leave as not to mess up the floor finish you might need to experiment with this depending on how accurate your machine is

Here are the settings I used for my test (your setting may vary but maintain the same chipload)
RPM: 18000
Feedrate: 150 ipm
Plunge Rate: 40 ipm
Lead-in/Lead-out Rate: 150 ipm
Chip Load: .0028"
DOC: .75"
Stepover: N/A
Cutting Direction: Conventional and Climb

Remember your chipload formulas and always check your tooling manufactures chip load recommendations when programming to insure warranty and tool life if you cannot run at these setting then adjust accordingly to maintain chipload

So as far as cutting direction goes conventional or climb it really does not seem to matter a whole lot you can get tearout on both and you can get clean finish on both. It just seems to be whatever mood the wood happens to be on that. I need to do further research on why that is. In my experience however you want to Conventional cut outside profiles and Climb cut internal profiles when finishing. When roughing I would just run conventional all the time

So following these different suggestions lets see what we get right off the machine shall we?

Here is what the piece looks like overall after all machining was done there was not sanding or post processing done

Showing here is the inside pocket that we made I used climb milling here and got a glass smooth finish on the edge even through the knot

Here I am showing with the grain cutting I used climb cutting here as well and the surface finish is glass smooth and no tear-out

So on this circle I used climb milling on the outside profile and you can see that we have fuzzies but these can be taken off with a quick 220 grit paper

This was the best out of them all no tear-out and no fuzzies I used conventional and ran finishing at full depth

So on this circle I used climb milling and also a ramping toolpath which you can see a faint line off where the tool ramped down

Here I am showing the cross grain finish and I think it turned out pretty well and there is minimal tear-out

Here I am showing the floor finish the floor finish is a little rough and you can see some tear-out but the point of this test was edge finish no floor finish and this is to be expected with a single flute tool to clean up the floor you can use a 3 or 4 flute flat bottom endmill and clean it up ASAP

I hope this helps with your pine routing adventures

Also note that Pine/Douglas fir lumber like any wood will change with humidity and temps so once you are done routing be sure to seal the wood as even within a matter of hours your fuzzies and roughness can come back


That is quite the write-up! Thank you!

Your welcome I was just having a little fun in the shop today for a upcoming job and I though I would share my results and experiences lol

1 Like

today I might work on floor finishes but I really need a flat endmill with radius end

this thread is discussing a material specific application so the machine you use does not matter

also please note my disclamer

“Remember your chipload formulas and always check your tooling manufactures chip load recommendations when programming to insure warranty and tool life if you cannot run at these setting then adjust accordingly to maintain chipload”

yes I did use my larger machine to perform this test

Hey @WorkinWoods it could be confusing for people reading this if you did not use the X-Carve especially since you show the X-Carve clamps in the picture. Can you please either remove the post or update the settings in the original for an equivalent test on the X-Carve?

Also the largest bit that fits in the Dewalt 611 is 1/4" but this bit is larger.

I think this post might be better for the forum of the machine that the test was done with.



sent you a pm

Hey @WorkinWoods read our latest PM but I don’t see the update. What am I missing?


This calculations where made with a unit power factor of .25 and thats for aluminum pine wood is much softer than aluminum

Tool 1.

Within the hp range of the x-carve

Tool 2.

Within the hp range of the x-carve

Have you tested a .250 depth per pass on dimensional lumber? It seems too deep based on my experience.

Also I think the RPMs might be too fast. What number do you have the Dewalt on?

1 Like

Speed 1 on the Dewalt 611 should be in the 16,000 rpm range.


yes I have cut that deep on the x-carve in


if you feel more comfortable run at a .125" doc but remember after the initial slot has been made you are only taking .0825" radially as you step over with proper machining strategy

For advanced software other than easel you can use trochoidal milling you could plunge all the way to .75" doc and bore through the material creating a slot if you use the correct optimal load settings

its really all in how you approach the toolpaths and the material

for the speed we are using a single flute tool so to maintain chipload we can speed the router up setting 4 should work nicely

for the 18000 rpm setting we can use setting 2

and also if you have a speed controller you can really dial in your speeds

please note that the fixture has alot to do with is which I did not explain in this specific post

but you need a rigid clamping and stop blocks and a finely tuned x-carve with the Dewalt not the quite cut spindle

What do you mean by the fixture? Your picture shows the wood clamps we sell.

A few minutes ago

2" pocket at 150 ipm, .25" depth per pass, .25" 2 flute up cut and the X Carve zipped right through it. I prefer to run a little slower but there were no errors. The machine was flying at 150ipm.

Yeah for the little test that I did the clamps work fine

I guess I mis-spoke there they are not considered a fixture that more of a clamp

but for the x-carve I would recommend a combination of either

clamps and screws
clamps and dowels
clamps and stop blocks
composite nails and stop blocks

for running the test you can just use clamps as a non rigid setup is pretty easily shown in a finishing pass as lines or waves

but for sure I would love to do a post on all the ways to clamp and fixture a work piece but that would be a long one to say the least

but in my experience on the x-carve the more you can do to make your setup and machine more rigid the better

very nice!! gotta love the speedy cycle times on parts

did you ramp in on that? or plunge straight down?

2" circle in Easel and cut.

Right now I am completely stock but I have Charley’s Y plates and have been eyeing the linear z everyone is playing with.