Can I speed up my carve in oak?

Some simple holes cutting into some oak but it says it’s going to take 1 hour 30 mins!? Can this be sped up? The depth is 20mm (0.79") with a diameter of 35mm (1.38"), I planned on using a 1/8" straight cut as it’s the most robust and biggest bit I have.
Could someone help with the Feed, Plunge and Depth values? There has to be a fast solution??

You can go to custom settings and do it there or during the carve on the top bar you can do it too

Oh I know I can change them in custom settings, I just haven’t got a clue what they should be. I don’t want to snap a bit or do something worse.

During the carve you can speed the rate up and see the results immediately

I do play around with the + and - sometimes which does bring the time down.
Would you change the depth per pass in my case? I’m not brave enough to play with that option.

I wouldn’t with Easel generated toolpaths. If you’ve adjusted your feed with the overrides, then you should have an idea on where you can start. I think the best option would be to get a 1/4" end mill.

1 Like

DOC is recommended at 1/2 the diameter and you are right there. 50 ipm is about all I push it in oak.
Like Neil said get a 1/4" bit.

@AdamBeech. Take small steps. It also depends on the bit being used. Experiment in very small increments

I have broken several bits but ALL of them involved screw ups. You break bits when you error in the initial settings and jamb the bit in, hit a clamp or have the depth/speed WAY off (often a misplaced decimal point).

If you start the carve with the “suggested” settings and then start slowly bumping up the feed speed you shouldn’t break anything. Just watch the cut and listen the the router. Normally the first sign of problems is the bit will start to chatter. Still at that point it won’t break an 1/8" bit - just back off the speed a little and you are fine. You usually can increase the suggested feed numbers by a fairly decent amount.

With that said, you could save a lot of time on this project by doing a 2 stage cut using a larger bit for clearing/roughing. If you don’t have a 1/4" bit you need one. Also, inexpensive hardware store or lumberyard 3/8", 1/2" and 3/4" bits can be used for clearing. They may not cut the cleanest but for roughing out excess material they can work fine.

Thank you all for the responses. I’ve got some 1/4 inch bits, how do I tell easel that that’s what’s being used?

Select a “custom” bit, enter 0.25" as diameter.

I must’ve misread the original time is would take, it wasn’t 1 hour 30, it’s actually 2 hours 50 with an 1/8" bit.

@cg49me If I change the bit to 0.25" what should I change the cut settings to? If I leave them it says it’ll now take just over 4 hours.

I should have looked closer at your project. Obviously, a two stage carve is not needed.:face_with_raised_eyebrow:

In oak I usually don’t follow the suggested 1/2 of the diameter for the depth of cut. It tends to be a little aggressive for my machine. I would start at .08 depth and 80 ipm feed and adjust from there. Throw a scrap of oak in and try a small cut at these settings. You are in no danger of breaking anything running them and you may be able to push the speed as you watch the process.

At my suggested settings I am guessing about 30 minutes.

@AdamBeech You are removing quite a bit of hard wood…it will take a while. Is this a one off project? Can I ask what it is? There may be other ways (depending on desired outcome):
Based only on what I see in your screenshot, what if you profile cut some holes and then glued the bottom on? Maybe a drill press with a forstner bit…the CNC could spot some pilot points.

Feeds & Speeds.
I cut a lot of exotic hardwoods, harder than rock maple or red oak. For many projects if I can use a 1/4" bit, that is what I go for. In the metal machining world the machinist lives by the cutting depth and speed ratios provided with the tool - in this case the end-mill. With wood routers bits there is no data, but you can get there with some thinking.

Number of flutes. The more flutes, the more cuts per revolution. However, the more flutes, the shallower the flute for removal of chips. If you are using a single flute cutter, the flute depth will be close to half the diameter of the bit itself - no more then 0.40 of the bit. Deeper flute means more material removed per cutting edge, and more material per revolution.

Revolutions = that is the cutting speed. Metal mills provide the depth of cut and the cutting speed. The cutting speed is always IPM - not RPM. So you must apply math to convert the IPM cutting speed into a proper RPM. The faster the rpm, the faster the cutting speed.

Feed rate - you can start playing with this once you have determined the speed and depth of cut. I am going to use some simple numbers here for the concept. Let’s assume that the mill cuts. .01" per revolution. For each revolution the cutter removes .01" of material. At 100 RPM the cutter removed .01" X 100 Revolutions = 1" of material removed = 1 IPM feed rate. Now - the Dewalt spindle can turn between 19,000 - 29,000 rpm. Let’s assume we have it set for the slowest speed and the same bit, .01 X 19,000 RPM = 190 IPM. If we speed up the spindle to 29,000 RPM the feed rate increases - .01 X 29,000 RMP = 290 IPM feed rate.

That is the theory. Now enters the reality. The X-Carve machine does not resist torsional forces very well, it is too light and made of flexible materials. High RPM and High Feed rates introduce more flex to the machine, creating chatter and reducing the quality of the cut.

While many of the end mill bits we can get allow us to have very high IPM feed rates, the stiffness of the machine limits how much stress we can put on the machine and get a high quality cut. Get the RPM speed wrong, the feed rate wrong, or the depth of cut wrong, and you will either have a rough cut or a broken bit.

Things get more exciting if you are doing a plunge and cutting a single pass grove. The cutter is cutting across at least 160 degrees of the bit, if not a full 180 degrees. In most milling operations (metal again) or in progressive passes, only about 90 degrees of the cuter is in full contact with the material. It is these plunge cuts where w place the most strain on the machine, and if we get depth or feed speed wrong end up breaking the bit.

As a few rules of thumb - when I am cutting a hard exotic wood, I use 2 flute cutters, set the spindle to the slowest RMP and start with the recommended feed speed to start. I can change the RPM up at any time independent of the program controls, and can change the feed speed in the program while it is running. I listen to the machine, and step up the feed and the rpm until the machine sounds the same cutting in any direction.

One last comment. The machine is the strongest cutting in the Y axis, as there are two motors driving the machine in that direction. Also, int he Y axis, the deflection in the gantry and the z axis is irrelevant - will not alter the quality of the cut. So I will speed up the cut speed manually for the Y axis cuts. In the z axis, the flex in the gantry and play in the both the Z and X axis will introduce chatter, si I will reduce the feed speed and increase the RPM to reduce this chatter.


Very helpful, thanks a lot.

@NeilFerreri1 It’s an egg holder, someone on here was kind enough to send me a .crv of a curved base (3d cut) but the customer changed their mind and wanted it a bit different. I found this, much smaller, on the projects page and tweaked it for my needs.
The problem of time would’ve still been the same if it was a 3d cut.
I don’t have a forstner bit big enough but I have considered using a fluted wood bit for the same reason.

@AdamBeech I think I’d go with two pieces of wood. Cutting a hole by cutting out a circle is much faster than pocketing the whole thing. You’d und up with little cylinders left over rather than sawdust. Then glue a piece of maple or something with the small pockets to the bottom.
I hope that makes sense…I can throw an example together later if it doesn’t.

@AdamBeech - You are welcome Adam,
I use Fusion 360 for developing the CAM for about half of my projects. It does much of the math for Speeds and Feeds - based on the parameters for the mills. Fusion is Free to hobbyists and small businesses. It gives you ultimate design control - but at the cost of a steeper learning curve than Easel. Another good source of info is Bob Warfield’s CNC Cookbook web site. Take a looks there - remember that the site is for guys cutting metal - which is not all that different than carving wood. There is much to learn there that can apply to the simple X-Carve.:sunglasses:

It’s not what I really wanted to do but I think you’re right, the labour involved in using the X carve to drill all that out is basically a waste of time. Doing it your way makes much more sense.