BIT BIBLE IDEA: Video archive and book showing every bit and result

Ive been looking for some kind of image or guide that would show every bit, how it cuts, and the finished product but I have not found anything that would satisfy my own desire for knowledge and design standards.

Ideally what I envision is as follows:

  • A large printed poster 40x60 that shows every bit, with its name, details, size and SKU
  • A web based searchable mobile/responsive version with links back to the inventables store of course…
    (I am a PHP web developer, so I could do this easily)
  • A printed “Bit bible” - book version showing the same info as the poster
    (I would use and InDesign, likely 12x12 hardcover)
  • Next to each bit image- photos of the cut/carved material from the top (and several other angles)
  • Videos for each bit on a youtube channel
  • On each bit I would test:
  • 2 | 4 | 6 speed
  • 1/8 | 1/4 | 1/2 dpeth
  • Plastic | Wood | Ceramic
  • = for a total of 12 samples of each bit

I am open to planning here, so if you have some ideas on the “result matrix” please let me know.

So… I am wondering, before I embark on this huge time consuming (and expensive) endeavor…

#1- has anyone put anything together like this? If so, can you share the link with me?
#2- If not, would anyone like to have something like this? If so, I am considering ordering 1 bit every week and producing my own Poster and Set of Videos to share with the community.

Notes: I’ve seen this: Color coded Inventables bit guide
and its cool, but not visual enough for me…

I’ve also seen this:
but it lacks what I feel is a much needed BIT ONLY guide dedicated to showing the end result of the cuts on various materials, depths and speed.

If there is no interest in this concept then I will create something that’s only useful to me, but anyone who wants something like this done, please comment and “vote” for it to let me know there is an interest in this. If I know other people would want this it will change how and what I produce.

My goal is 2 fold, first off the knowledge I would gain would be worth it, but secondly, to be able to transfer that knowledge to others by documenting the process I feel would be helpful.

let me know…

1 Like

There have been a couple of efforts by Inventables toward a similar goal:

…but they aren’t as complete (yet?) as what you’re proposing. I’d definitely be interested!

Certainly a humongous venture … sounds interesting. Wish you luck on it … Just curious, what speed do you run your router on currently? I dont have a 9 on my router…

I assume you’ll be using your Xcarve for the pictures so others can follow along … (?)

1 Like

[quote=“ChristianWZagarskas, post:1, topic:59798”]
Ive been looking for some kind of image or guide that would show every bit, how it cuts, and the finished product

The Bit Bible, Vol 1


yea… saw that one… few things about that video…
first time through it was ok, I absorbed some useful info.

but @35 min - quote "ive got a few more images to show you guys, hopefully this is interesting, i’ve no idea. um, hardwoods, a little bit different than the plywood…" and then drops a couple jpg’s onto the screen

I felt the video was done to fulfill a request at work by someone who did not really want to do it, much less do it well. That is one of the things that inspired me to write this post in the forum.

It seems to me that this is the only resource that inventables put out on this subject?

maybe this is common knowledge to pro’s, but the xCarve seems to me not to be marketed at people who are using ProEngineer…

seems to me that the only way I am going to learn is to load up 100 bits and waste some materials doing tests. I might as well document those tests for the sake of posterity.

I figure this will be a good way to get a feel for the community here…

@AkamaiWoodworks - I am having trouble seeing how your post contributes to this conversation…

I think so. what do you mean exactly by “using your Xcarve for the pictures”. this makes me think there is some kind of video camera attachment that I should look into? Is there one? Please elaborate.

As for the settings, yes, it only go’s to 6. It is a Dewalt 611
I was looking at the table upside down and thought it was a 9

It was a joke on your comment that your guide would show EVERY BIT.

Since there are so many bits and all the criteria that you intend showing for each one, your book would be HUGE!

1 Like

I have done something very basic and with only three different bits. I would refer to something all inclusive like this all the time. This would be extremely valuable.

That’s a hilarious picture, Akamai.

There would be a lot of value in this. It feels to me more like a wiki than trying to do a poster. People can add images, video, tips, tricks, etc. and it would be searchable with crosslinks, etc.

That said, I have no idea how to get started on something like this!

I just want to also say that there are software tools available that can model most every type of tooling and it’s interaction with most every type of material on most every type of CNC setup. This allows CNC users to very quickly and precisely determine Feeds and Speeds for the bits and materials they want to use. Software like this can determine the difference that 1 inch stick out distance of a tool would have vs 1.5 inch stick out. It can also take into account the power of your spindle and the stiffness of your CNC. All of these variables can make a considerable difference in how a specific tool behaves on your CNC machine.

In my opinion a catalog (Wiki) is great for general guidance and understanding the major differences in tools (Upcut/downcut, endmill/ballnose etc…) But trying to document every tool with every material at every feed/speed seems less useful to me. Of course I could be wrong, since I have not seen the document you are describing.

Example of software tool (The only reason I link to G-Wizard is that I use it and find it very valuable, I have no relationship with the company other than as a customer)

So I’m an engineer by trade and here’s my perspective on this approach and why it would end up being a waste of time, money, bits, and material.

It boils down to way too many variables that you could never actually complete this project nor get results that are worth looking at.

  1. Not every bit type can be documented for use on an Xcarve, they just don’t fit into the Dewalt or the Xcarve just isn’t rigid/powerful enough to actually see the benefits of the bit type. And so a 4 flute chip breaker bit may end up being exactly the same as a 2 flute downcut.
  2. Every material, even the same species, won’t be the same cut. We’re talking primarily about wood here. I can go buy 2 pieces of pine and each one will mill differently. Knots, oils, resins, moisture, etc. You could easily try 20 different pieces of pine and never get the same results.
  3. Bit material/coating will alter results. Solid carbide versus carbide tip versus HSS versus ALTIN coated versus TICN coated versus Spectra coating.
  4. Bit sharpness. The quality of the cut and finish will change as the bit dulls so to truly do this, you need to take each bit from fresh out of the box all the way down to dull on each material and each setting and each speed.
  5. You can’t expect the Xcarve to perform the same as a commercial CNC. You will inherently get variations because it is a hobby machine. That’s not saying you can’t get good results but what you’re wanting is outside the realm of expectations.
  6. You mention 2/4/6 speed. Why not 1/3/5? Considering the vast majority of Xcarve users should never move their Dewalt off of speed 1, why even test other speeds?
  7. Commercially produced router will have different run out values for each router which changes the cut.
  8. Router collet tolerances can affect run out which affect the cut.
  9. Router wear and tear during testing will change the run out and change the cut, so you’d be constantly changing your router to a brand new one
  10. Inherent vibrations from cutting will loosen parts on the machine affecting rigidity and cuts so you’d need to rebuild and re-torque your machine multiple times to keep that from happening
  11. You mention depths, are you referring to multiple depths of cut or total cut depth?
  12. Bit deflection will play a part so you’ve got to vary your feed rates throughout all of these tests.
  13. Amount of the bit sticking out from the router will change the cut performance.
  14. Toolpath strategy changes the cut. Conventional vs climb milling. Offset vs Raster.
  15. Bit supplier A vs supplier B will have different cut finishes for the same type of bit. 30 degree Vbit from A might be 29 degree from B.
  16. Machine to machine variations. My machine was built by me. You built yours. Mine might be built better or it might be worse. That will change how cuts will be.
  17. OEM collet versus Elaire collet versus PreciseBits collet

I could keep listing variables all day long but in the end, there’s absolutely no way to control them all.

My recommendation? Find a bit supplier that you like and explore the bits they have for your needs and stick with them. Whiteside makes good bits. I like using Kodiak Cutting Tools as well.

Also, a word of advice, stop over thinking using the Xcarve. I used to do that. That’s why I’m a pretty good engineer, I analyze everything too much. Just use it. Figure it out. Understand you may trash a $30 piece of maple because of a bad setting. As long as you learn from your mistakes and grow, this stuff will come natural.

Things like surface finish or pocket bottom finish or chamfers or whatever will come with experience and time.

Just carve stuff. You’d spend years compiling all this information and then realize you’ve never used your Xcarve for fun.


If this is not done too in-depth it could make a useful chart.

But as many others have said running every bit at every speed at every feed is overdoing it, because you’ll find that 90% of your tests will consist of unusable settings.

But I think most of us have at least a file somewhere with optimal settings for different materials. You can never go wrong experimenting and sharing your experience.

Learn as you do projects, don’t make this into a chore you need to go through. Keep it fun!

I think @JustinBusby is 100% correct, it is very tempting to overthink your feed and speed settings. The best advice I ever received on this forum was to trust these rules of thumb.

  • Keep the Dewalt RPM speed low (1) - I did not believe this till I did the math and proved it to myself
  • Keep the Depth of cut to about half the tool diameter
  • Use the largest diameter tool that will work (Stay away from those 1/32 bits, use a tapered or vbit instead)
  • Start with a feed rate of 60 ipm and see how it does

Starting with these basic rules you can be pretty sure you will not break to much stuff, then you can make minor tweaks as you watch it cut.


The amount of variables are simply too many for this endeavour to be universal. You can get a good baseline on yours but every other machine out there will be slightly different.

My advice for all is to learn to use the end mill information from the manufacturer, this is the baseline they provide for their tool and is often a sound starting point. They do assume a commercial machine so achievable Xcarve numbers may be less - But learning where to go gentler with a less rigid machine is key

There are three main factors to be considered:

  • RPM (in relation to ideal cutter speed)
  • Chip thickness / load per tooth (how much does it need to bite in order to remove material efficiently)
  • Feed rate (this is governed by RPM and Chip thickness)

I often visit this one to get a baseline:

First I determine the RPM I want to use (Say Dewalt #1, 16k RPM)
Then which end mill, say 6mm 2F
Material is wood, suggested chip load is 0.09mm/tooth

Feed rate => 16k * 0.09 * 2 (teeth) = 2880mm/min (113IPM)

The last variable is the depth per cut, this is governed by the rigidity of your machine and ultimately decide the achievable material removal rate (MRR)
Start shallow and increase until you feel max is reached. This will be your maximum MRR, reduce that someone for a consistent result.

MRR = Feed * Width of Cut * Depth per Cut
So if you try 0.5mm DoC you get: 2880mm/min * 3mm WoC * 0.5mm DoC = 4.32ccm/min
If that is too aggressive for your machine, reduce the depth per cut or step over, dont reduce feed rate/RPM since that need to maintain a decent chip load otherwise it will rub/heat up and go bust.

“Keep the Dewalt RPM speed low (1) - I did not believe this till I did the math and proved it to myself”

This boggles my mind but I’ll try it. I do bump down to for for plastics but back up when doing wood. Your saying always a 1?

Yes, 1 is always the speed to start with. If you are using a large diameter tool with a single flute then maybe 2. Or if your feed rate is much faster than normal then maybe 2. The problem is that at setting 1 the Dewalt is spinning at over 16,000 RPM which is very fast.

Honestly the Dewalt is halfway up the speed spectrum for most of the bits inventables sells. If you have the ability to drop to a lower speed you would do it on 80% of your jobs. That’s why I switched out to the Makita.