Cutting through Soft Maple

I’m using a Carvey, and the Aspire 3D software. Although what I’m attempting to make has nothing to do with actual 3D modeling, or anything like that.

Using a .25 inch end mill, (shank & diameter) (2 flute, up cut) how long do you think it should take to cut two round blocks, each 2 inches in diameter from a piece of soft maple that is 3/4 inches thick?

I ask because I’ve been trying to make this box for over a week and a half, and so far everything goes fine until it gets to the profile cut to cut the actual bottom and top pieces out. I have tried a vast multitude of settings, but each an every time, it gets hung up, and deflects, and is just all over the place after that. My last attempt the settings were set to

Pass Depth 0.03
Stepover 10%
Spindle Speed 12000
Feed Rate 30 in/min
Plunge Rate 9 in/min

Est Cut Time 2:06:22:

It made it about 3/4 of the way through when it just hung, veered drastically off course, and caused an error to pop up in Easel about the spindle being over worked…

I am apparently either doing something obvious yet significantly wrong, or I am cursed at working with CNC and/or wood.

As I have said, I have tried a multitude of settings… faster, slower, higher, lower, deeper, shallower… Some get further than others, but eventually, they all just hang or deflect significantly off course.

Supposedly the Carvey can cut a piece of wood 2 inches thick, and sometime even 3 inches depending on the cut. But I can’;t even get through half inch soft maple.

My pocket carves, and the profile carves for the lips all work great. Just cutting them out of the block is giving me fits.

What should I be looking at? I’ve been trying this for so long, I’m at the point of just trying random settings. I’ve gone through so much wood trying to get this thing made, it’s costing me a small fortune. I suppose I could set my pass depth even shallower, but at 0.03, it’s already a two hour cut for something that should be a whole lot quicker.

I can attach the aspire file if it would make any difference, but from what I can gather by reading the interwebs, this should be a fairly straight forward cut. I can go to a smaller bit, but to make such a small box shouldn’t take hours to cut on a CNC, should it? What’s the average length of cut time for a .25 end mill, .75 inches of wood?

Based on the settings I specified in the OP, here is an image of where things went awry in my last attempt. As I stated, the pocket and profile (lip) all cut fine. But the profile cut to cut the block out is where it failed


None of your settings strike me as being red flags. I think you’re good on that front. I don’t own a Carvey however so I’m not fully aware of its capabilities and shortcomings. I don’t see the point of the 10% stepover value though if you’re not working a 3D file. You should ramp that up to 40 or 45%, which is pretty much standard.

I’d do the profile cutout with an 1/8 inch (same settings) and see where that gets you.

The difference between your pocket and profile is obvious:
Pocket cut with 10% stepover and a 0.25" end mill means 0.025" material engagement.
Profile cuts are always 100% by definition so 0.25" material engagement, which is ten times more.
so the fact you only encounter problems on a cutout is perfectly logical.
Are you clearing the chips? This can be very important on deep slotting.

With problems like these, pictures always help :wink: (edit: I see you added one :+1:)

As I said, I’ve been at this for about a week and a half, so every setting within there has undergone significant increases and decreases. The step over setting was just one of the latter ones I was changing at random, which is why it was there. I would normally have it at 40%, but I was trying everything I could think of.

I had started with an 1/8 diameter end mill first, but was thinking a bigger bit would clear more out in each pass, and should therefore be quicker. I’m down to only 2 more .75 inch maple before I suppose I’ll just give up. But I’ll try one more with an 1/8 bi on the cutout path. At this point, it surely couldn’t hurt.

If the end mill isn’t truly perpendicular to the X/Y plane the skewed/raked bit will face more problems deep vs shallow.
Chip clearing is imperative.

It may be simply taxing your Carvey MRR (Material Removal Rate), trying a 1/8" may be next step.
With an 1/8" up the step over to default 40% and you could maybe go slightly deeper per pass.

You pocket data = 30ipm x 0.03" x 0.25 x 10% => MRR=0,0225ci/min
Contour data = 30ipm x 0.03 x 0.25 => MRR=0,225ci/min
I suspect this is quite a load for the Carvey.

Running the 1/8" at 40% step over and 0.03" depth per cut give a MRR of 0.045ci/m.
So effectively it should do the inside in half the time.

1 Like

One of my first tries was with an 1/8 em for the pockets, and it resulted in a cut for 1:27:46, but when I switched to the 1/4 em, it went to 00:41:35 which is why I switched everything to the 1/4 bit. But perhaps the 1/4 is a bit much for the Carvey, I don’t really know, I’m guessing and reading stuff online, trying to figure all this out. While they claim the machine is capable of using it, doesn’t really mean one should. I’ll leave the other cuts at the 1/4 since they do work right now, try the final profile cut with the 1/8 and hope it goes through.

Thanks for your responses and help…

A 1/4" but does remove more material, but it’s harder for the little spindle to turn. I’d stick with 1/8" shank end mills. How deep is the cut when it goes off path? Are you sure you’re not hitting the collet or a plastic ring on the end mill?

No, I’m sure it’s not hitting the collet, nor the end of the bit. It’s usually about 3/4 of the way through it’s cut when it seems to struggle for a second, then boom off course or I get the Easel popup about being overloaded.

I’m re-trying the 1/8 bit now. It’s going to take a little over 2 hours. I was hoping I could get some better performance, but if it finally cuts through, I’ll consider it a success. At this point, any success will give me some hope. :slight_smile: From there, I’ll start playing with those settings a bit to get a clean cut, but maybe a bit more speed out of it too.

Looks like I need to get more wood. I tried MDF to save a few bucks, but I hear it’s bad for bits, and I’m not too keen on it’s look. I’ll let you know if it works out for me. And again, thanks.

Open it up and vacuum every once in a while.

Pine and poplar are relatively cheap. At least they are in Ohio.

1 Like

I did. Probably more than I really needed, but I did. It finished, and after a little bit of sanding, I have what I intended. Lesson learned, stick to the 1/8 bits. Remove waste material frequently, and be patient.


I dont know Aspire as I usually work in Fusion360, but different tool path strategies can have a huge impact on achieved MRR and therefore time required. Going down in 0.03" increments you only use the 0.03" tip of your tool, choosing a tool strategy that allow a gentle helical plunge to say 0.2" depth with a outward spiralling motion to clear that level of material. The step over is set to keep whatever MRR within limit of your machine.
Upside is you use more of the tool cutting length => more even wear and longer tool life.

Here is a descriptive video on this topic, Aspire may have something similar:


I was able to finally cut this out, sand, and stain it. It’s a little sloppy looking, have to get better at my sanding and staining, but overall, I’m still chocking it up to a success.