Repeatable process for setting Feed Rate and Depth of Cut in Easel and elsewhere

I’ve been trying to understand feed rates and depth of cut settings in Easel, and eventually for Fusion 360.

On my first set of cuts I burned out a bit cutting some Oak.
On my next set of cuts I snapped a small bit trying to push it too fast through some aluminum.
Clearly you have to know this stuff to get it right.

@AllenMassey had a great spreadsheet that calculated RPM settings, which taught me a lot,
but I am using a deWalt and the advice I have seen is to keep it at the ‘1’ setting, which is fixed at ~16,200 RPM, so I needed a way to use that data to calculated a feed rate instead.

I added a tab to the spreadsheet to calculate feedrate basedon a formula I found,
and discovered that at 16,200 RPM the minimum feed rate using a single flute tool (unlikely) would be ~48 IPM for a material like hardwood, if you trust the calculation:

I then wanted to understand how that lined up with the defaults that Easel uses today.
I did a small data gathering exercise by going into the settings tab in Easel for various materials and bit sizes and discovered that where the spreadsheet calculation distinguishes between number of flutes and chip load based on material and tool size to ramp up and down the feedrate, it appears that Easel today uses static materials-based values to set this:

As a point of comparison, then, where the spreadsheet above says that Hardwood should have for a single flute 1/8 bit a feed rate of ~48 IPM, the Easel default for ‘Hard Maple’ is 28 IPM. This seems like a big difference.

In previous discussions in the forum where I have asked some questions about this, I have had people advise that it is best to get ‘as close to 60 as possible’, and that the best way to set this is to experiment with test cuts. This is fair advice, but how to set even the initial values to test with? Surely we can do better than guessing?

Since I am new to the XC, I have a fundamental question related to the capability of the machine. People in the fora say things like ‘the XC will not push through material that fast’, hinting there is a liimit to the lateral force the XC can provide which will limit the feed rate that we can request and productively receive.

Having gathered this data and these impressions, here is my question:
is there a way to generate a data set we can use in this spreadsheet CNC Speed Calculator for Dewalt.xls (75 KB) to reliably calculate a feedrate value for an XC with a deWalt head which will provide optimal tool life and cut quality, within the limits of the XC machine?

options might include:

  • a max feed rate value for a tool size/material combination that could be used to override the calculation
  • a pro-rate value, specific to the XC, applied to ‘adjust’ the feedrate in some way. Again this might be material and tool specific… but also an alloowance for what the XC can and cannot do…

Many people here have the ability to contribute experience about what final values might look like that appear ‘right’. I know I’m going all six sigma on you, but I am hoping to find a way to gather that community experience into some form of reliable and repeatable guidance that could be used in a variety of circumstances to the benefit of people like me who though lack of experience are not yet capable of such feats.

Thanks for reading. All advice gratefully received…


The actual limits of the X-Carve are the defined by the power (torque) of the spindle, the power of the stepper motors and power transfer limits of the pulley and belt drive and finally the rigidity of each of the mechanical portions of the machine.

I have not performed actual load cell measurements but in my experience the second most limiting factor (at least on my machine) seems to be the power transfer function from the steppers to the carriage. It is possible to “stall” the carriage when under heavy load. Either the steppers are not providing enough torque, or the pulley will slip on the belt (or the belt will break). Exceeding this limitation will cause the X-Carve to immediately loose steps and or damage the belts drive.

The next largest limitation is the ability of the mechanical system to resist deflection at the end of the tool. If the drive system was able to provide infinite torque at some point the force applied to the tool tip would cause the spindle to deviate from being perpendicular to the work surface (it would no longer be normal to the work surface). On my machine this is the primary limiting factor since the spindle will begin to deflect before the machine stalls and looses steps. The force required to deflect the spindle can be increased by reducing the stick out of the tool (reducing the leverage arm) but eventually with enough force supplied by the motors it is possible to cause deflection. For some jobs a small amount of deflection is not very noticeable, for other operations it may ruin the work.

Fortunately there are ways to minimize deflection (like using conventional instead of climb cutting), or just slow down the feed rate. Here is an excellent article about this subject from the CNCCookBook.

This is why the stiffening mods are so important. The stiffer the frame and carriage the more force that will be required to deflect the spindle. Increasing the stiffness of the frame and carriage until the motors are not capable of causing deflection would be ideal. Then the limiting factor would be the torque of the motors and the ability of the drive system to transfer that power.

The last limiting factor in the power available from the spindle itself. In my experience the Dewalt 611 is capable of providing more than enough torque it has never been a limiting factor on my machine (except for it’s inability to run below 16,200 rpm). This rpm limit of the Dewalt causes the optimal feedrate (based on recommended chip load) to exceed the other limiting factors of the machine (primarily deflection)

So where all this has lead to is that the X-Carve may not be able to achieve optimal chip loads using the Dewalt 611, if that is your primary goal then you would be able to get much closer by purchasing a VFD Spindle and inverter, that can run as low as 6,000 rpm. If you put 6,000 rpm into the spread sheet you will see that the recommended feed rates for most tools and materials are within the operating range of the X-Carve


@AllenMassey very thorough and excellent description of the challnege.
for sake of argument, let’s pretend I am committed to the deWalt, at least for the next budget cycle.
how would I systematically and repeatably optiomize my settings given what I have?

Well the first thing is to ignore the recommended chip loads, you aren’t going to get there.

Keep the Dewalt speed low (near 1)

Keep your depth of cut conservative no more than half the diameter of the tool. Reducing the DOC will always allow you to increase feedrate, but if the DOC is to shallow you are doing more rubbing than cutting and that is very bad for the tool. So the half diameter rule works pretty well.

Use sharp tools, carbide is always best, try some two flute straight flute cutters they do a really good job. Even with spiral cut try to use two flute tools, the more flutes the worse your chip load becomes.

Experiment with the feed rate and see how fast you can move through your material without losing steps and get a nice clean cut with no burn marks. For my machine I have found that if I can keep the feed rate around 60 ipm I can get nice cuts with out any fear of losing steps. Your machine may be different, the only way I know to find the sweet spot is to get some scrap material and make some cuts (profiles and pockets) and see how high you can push the feed rate before you lose steps or the tool deflection becomes noticeable.

I know that is not the greatest of answers if you were looking for exact numbers, but that is all I know to tell you.


x-posted to Autodesk Fusion 360 forums at

This post is going to sound like I do not like the X-carve, while I actually love my machine and find it very useful. I was very aware of it’s limitations before purchase and do not mistake it for a machine that costs hundreds of times more than it does.

The simple and harsh fact is that the X-carve is too weak in almost every aspect to do its job efficiently. I know I sound harsh but it is true. There is a reason why quality CNC machines weight many thousands of pounds and have the strength to snap 3/4" dia bits like toothpicks if crashed into the work piece. Rigidity and power are the only way to get good clean cuts; unfortunately, the X-Carve has neither (actually it is worse than that because we pair it with high speed spindles that only work properly if we can feed them at proportionally high speeds). In the real world the solution 9 times out of 10 is to either feed the tool faster or turn the spindle slower and these are the two things that the X-carve can’t do. So with that said there are obvious limitations to the machine and many of the existing tips and tricks on how to dial in feeds and speeds do not apply to the X-carve.

It is even harder to make claims as a whole on proper feeds and speeds because people have various sized machines (mine for example is 12"-X by 24"-Y) some are stock and some have extremely elaborate (and sometimes nonsensical) strengthening modifications. There is even how clean and well calibrated the machine is, one person might have their eccentric nuts tightened to the point the steppers are almost stalling and someone might have them so loose there is free play in the system each will result in different problems (one will stall sooner and one will chatter sooner).

At the end of the day to get the X-carve’s feeds and speeds dialed in it takes a solid personal understanding of how the tool is behaving within the substrate and knowing what the limits of the machine are and that sometimes its best effort won’t be good enough because the machine is not always capable of getting the proper chip load. You need to take big bites from the material to keep every thing cutting clean and cool but that takes a machine that will not flex and power to keep it moving smoothly and consistently. Taking a shallow depth of cut will solve many of the X-carve’s short comings but at the sacrifice of tool life and a large increase in cut time.

So… I got on a little bit of a rant here so to the original question, can we make a better process of calculating feeds and speeds on the X-carve? My opinion is a firm NO. I cannot calculate how to optimize it like I have done machining materials as the operator of much larger equipment, I instead need to rely on my experience and trial and error to get it to a point that I am happy with and that is still not always perfect.

I still love my X-carve but I know what I can and can’t ask of it.

1 Like

This is an interesting topic, thanks for posting it. I hadn’t realized that I needed to run my Dewalt at its lowest speed setting. Is that true even when using 1/4" bits, or just 1/8" ones?

I wonder if there is any way to slow the deWalt down.
I know there are rheostats designed for fireplace fans which will slow them down without burning out the motors through low voltage.
I wonder If you could use the same sort of thing ona dewalt to get it into the 5k-8k RPM range?

crossing streams again

I mounted a Makita router on my XC as it’s lowest setting was 10K RPM. I have never run it higher than #2 setting which I think is around 13k RPM.

It is all proportionally though and all works against the XC. You need slower RPMS to take thicker slices of material to keep the tool cool and the cuts clean. Our router spindles can’t do this and we also need a machine that is rigid enough to not flex as the cutting tool is cutting a thicker slice. I have wondered if a DC spindle will do the job but without the rigidity being increased I think you will just flex the machine more at slower RPMS. This is why people have the tendency to ramp up RPM to the moon because you are taking microns off the material per pass and not exerting any lateral force against the cutter but you are melting substrate and burning bits.

stream crossing back:

from another discussion:

if you think of feed rate, depth of cut, and spindle rate as an iron triangle, all inter-related,
then I guess it looks like this:

  • The spindle on a deWalt goes at 16k RPM minimum.
  • The feedrate for a spindle at that rate is unachievable, so go as fast as you can: in a hard wood the target rate is somewhere around 60 inch per minute if that is achievable
  • to push the spindle faster, make depth of cut shallow. The rule of thumb is half of your tool diameter: for a 1/4" bit use a 1/8" DOC, and do so on.

The easel program uses preset feedrates and DOC based on the material.
these are in the spreadsheet.
I am still trying to make sense of them;
they seem arbitrary if you consider material hardness to be important.
for instance, here is a list with the hardness rating for the woods:

Two woods with very different hardness ratings will have the same settings.

Does anyone have any idea how to make sense of this data?

1 Like

Thanks for the very useful discussion. Understanding that I am late to the party and am a newcomer to cnc machining, I would like to note that I broke down and bought the superPID speed controller, which allows the DeWalt router to operate at speeds as low as 5000 rpm without reducing its power/torque by imploying a pwm algorithm. To date, it has worked flawlessly. Expensive, but IMHO well worth the money.

do you have a link to that?
I’ve never looked at one…

Here is the link to the superPID. I really like it.

did you need to void your warranty to hook that up?

I did. I didn’t consider it to be a big deal, as the router isn’t very expensive and what you end up having to do is pretty simple and can be undone without much difficulty. I ended up taking all of the router electronics out and connecting the led’s to a remote switch so I could control them separately (a version of something I saw in a separate post). I really like my setup, and can try to take and post some pictures if you are interested.

Pictures would be great, thanks!

Sorry for the delayed response. Work temporarily displaced my hobby time (I hate that). I will try to post some pictures in the next few days.