Chipload and X-Carve Expectations

Hi Everyone,

I have been looking at Chipload figures for the types of cutters that might be used on the X-Carve and have had support from the Whiteside Machine Company. I have also looked at various threads on this forum to discover the theoretical maximum X-Y speeds possible and the practical expectation based on user reports.

From this I have produced a spreadsheet which may serve as an indication of what an X-Carve might be able to do. I do not claim that my work is definitive and must warn everyone that looks at it that their particular X-Carve may be better or worse than these figures predict. So please do not dial in any of these figures unless you are satisfied that your machine is capable of performing at that particular rate with whatever cutter you choose.

Here is the spreadsheet.

Chiploads New Brit Workshop.xls (36.5 KB)



Any ideas where would burrs fall on this chart? I cant even start to comprehend what chip load if any applies to them. I managed to start nice fire in MDF with this 1/4 baby …

1 Like

As far as I know there are no chipload figures for rasps. By the look of the one in the picture it would deserve a very low chipload figure as one should not expect much from it. The cutting edges are just ordinary steel with no hope of staying in temper from what you say so that too is working against you. It may be time to upgrade !


If I am reading your chart correctly it says that for a 1/4 inch compression bit with the Dewalt set at its lowest RPM of 16,000 (1) my feed rate should be 162 mm/sec = 385 in/min.

This would mean it is impossible to use a 1/4 inch compression bit (with a decent chipload). But I do it all the time at a feed rate of 40 to 50 in/min with good results. So I am confused about what your chart is showing.

Hi Allen

I have used the Chipload figures provided by Whiteside and they do seem to compare with example figures that I have seen elsewhere on the web. I have not checked out other manufacturers Chiploads for their 1/4" compression bits so that might give a clue.

As a general point I would say that the X-Carve, as an entry level machine, cannot be expected to perform like a $7,000 machine. The practical expectation figures are based on seeing someone say that they could not go over 74 inches per minute on their machine.

What would be useful now is for people to post replies to this thread with what they have achieved stating:

  • type of cutter
  • diameter
  • spindle speed
  • cut rate (either inches per minute or mm per second)

Also, if anyone has any Chipload figures from other sources that are wildly different from the one above then that would be useful to know as well.


Here is the chipload calculator I put together a few months ago

CNC Speed Calculator for Dewalt.xlsx (18.2 KB)

1 Like

Hi Allen

I am unable to open that file format as I am still using Excel 2003. Are you able to save it as an old fashioned .xls file ?



CNC Speed Calculator for Dewalt.xls (38.5 KB)

Hi Allen

Your spreadsheet has more useful numbers but now I am a bit confused.

The Chipload numbers that I used were just general wood ones that Whiteside had sent to me. In fact all of that area is just copied and pasted from their original spreadsheet, including the notes at the bottom.

Your Chipload numbers are slightly different from those from Whiteside. I have checked your source and you have made no transposition errors as far as I can tell.

Just how can the X-Carve be used with those figures because, I understand that cranking it up over 74 inches per minute causes problems. I have certainly not gone over 30 mm per second (about 72 inches per minute) as I think that is the limit of my setup.

Does this mean that Chipload figures are irrelevant as the X-Carve is not man enough to perform in the “sweet zone”?


(edit - I changed “quite” different to “slightly” different - oops ! )

There are several issues at play here

  1. Each bit has a unique chipload specification, but most of the bits I purchase from resellers do not include detailed specification (I feel lucky if the diameter is marked). So the “correct” chipload is just a approximation based on published data from other manufacturers

  2. You can make really nice cuts without having a perfect chipload, The perfect chipload will prolong the life of the bit and make good cuts. But not having a perfect chipload is not a huge problem (as long as the tool is being operated within reasonable speed limits)

  3. The lowest RPM the Dewalt will run at is about 16,000 RPM so we are already outside the recommended chipload range for feedrates that the mechanical stiffness of the X-Carve can reasonably support (less than 120 in/min)

  4. There are other factors such as Depth of Cut and the stepover that can have a much greater influence on the quality than chipload

  5. The diameter of the tool makes a huge difference, in general the larger the diameter of the tool the better. So I will always try to use a 1/4 inch tool if the project allows.

So based on that, what I learned from building my chipload based feed rate calculator is that the most important thing to do with the Dewalt is to keep the speed setting under 2 for most bits (there are some small bits and materials were it may be better to go to 4 but those are the exceptions)

Then with the RPM at 1, I start off with a feed rate of about 40 ipm and a DOC of half the tool diameter and then look at my results, If I am making several copies of the same project I will try increasing the feedrate in increments up to about 60 to see if the cut quality stays the same or not.

I don’t know about everyone else, but I think obsessing over used the “correct” feed and speeds is silly. Sure you want to be in the right ball park. But if you follow a few simple rules of thumb, the X-Carve/Dewalt will work well.

1 Like

Hi Allen


Many thanks.


upgrade? ummm just got it …
I guess you never used Burr bit before. They are usually to my understanding used for carbon fiber but it has been recommended to me for wood as well to achieve ultra smooth surface. I used it with success on both MDF and Ply.
I just feel like flying blind with the feed and speed using it.

Try running it a little slower as you said that you were getting some over heating. Try not to force it too much but keep it moving and see how that goes.

So, reduce the RPM and also the feed rate.


Hi (again) Allen

Would you allow me to copy the material specific Chipload figures from your spreadsheet in order to add them to my spreadsheet?

I intend to give mine away to anyone who asks and copy it to Whiteside.



Sure. I have been giving mine away also.

1 Like

Many thanks.