Posted by SainSmart on

Bit Dimensions and definitions

Your CAM software needs to know some things about the Bit to generate a toolpath, the amount of detail depends on the specific CAM software you are using. Things like the diameter of the bit are very important so it can work out how to cut out the shapes and contours you want. The shape of the bit is also important so it can calculate how deep it needs to be to achieve the desired contours, can it cut a vertical edge...


Shank or Shaft

The round piece at the top of the bit that goes into the collet, the collet size must match the shank diameter.


Overall Length

Length of the bit from top to tip.


Stickout (AKA length below holder)

How far the bit tip sticks out from the end of the tool holder. The maximum length that the collet will clamp is 18mm, the length that can go into the tool holder is ~25mm depending on the mounting. The Stickout and the positioning of the Spindle motor in the holder needs to be long enough to reach the bottom of the cut with the Z axis at its lowest and still to clear the top of the stock with the Z axis at its highest.

Keeping the Stickout as short as is necessary helps reduce flexing of the bit, increasing accuracy, reducing wear and the chances of bit failure.


Shoulder length

Especially in the case of small diameter bits the shaft diameter may be larger than the cutting diameter, the shoulder length is the distance from the tip this change starts. Effectively this is the maximum depth a bit can go vertically into the stock material, not as far as it can cut effectively though.


Flute Length

This is the maximum height of the working range of the flutes from the tip of the bit. This is not the same as the length of the spirals from the tip as these normally continue up a bit more than they can effectively work.


Maximum Depth of Cut (DOC)

Simply how far down the bit can effectively cut, this is normally the smallest of the flute length and shoulder length for a straight edged bit. If you are using a V-bit for example this would normally be the maximum depth at which it will cut a V before just starting to leave a round hole.  DOC is also used to describe the distance the bit is actually instructed to cut in a single pass but for a bit definition it’s the maximum depth it can cut.


Flutes (AKA Teeth)

The number of cutting surfaces on the bit. Used in speed and calculations to determine things like how big the chips are going to be and it will affect surface finish, speeds.....



The diameter of the cut or slot the bit will make, well not so simple in practice, what is the diameter of a V Bit? It changes from the tip to the top! This depends for some bits on what CAM software you are using.


Corner Radius

Normally applicable to bull nose bits, the radius of the corner between the tip and the side of the bit.


Taper and other angles

Just angles but depending on the type of bit and CAM software the angles can be expressed in different ways! Normally a V bit angle is measured by the angle of the groove it will make from edge to edge, often referred to as the Included Angle. But for a tapered bit it is normally measured between one edge and the vertical or the Half Angle.



The spirals on a bit have a simple job, to remove the chips away from where it is cutting so the bit does not get clogged. Something like a V bit doesn’t have spirals as the chips can just move away sideways or upwards by themselves.

But they may also come into contact with the side of the stock, so while they are not exactly cutting surfaces they still rub and so have an effect.



Where the spirals are shaped to provide extra cutting edges or surfaces to break up the chips more, or both. Think of a cob of corn but with sharp kernels arranged in spirals rather than straight lines.


Upcut, Downcut and Compression

This is all about the direction of the spirals on the edges of the bit. The edges of a straight bit will create friction from the rotating spirals and the movement of the chips and direction of the spirals can cause splintering on the edges of the cut, especially on laminated materials such as plywood or veneers and others.



The standard bit type, just like a drill the spirals move the chips UP away from the cutting edge. If a bit description doesn’t mention any cut type it’s probably an Upcut. Can cause a bad finish at the top of the stock.



The spirals move the chips DOWN towards the cutting edge, this means that the action of the spirals on the edge of the material is downwards which can help prevent splintering or the creation of a lip at the top, but if you are cutting all the way through a material can transfer the splintering/lip to the bottom surface.


There is a major consideration when using these in that the chips still need to be moved away from the cutting edges to prevent clogging. Having them leave at a side is the only option so don’t use them to plunge or drill into the stock!



Where you have a cut that using an Upcut bit leaves the top ragged but when using a Downcut bit leaves the bottom ragged. Use a compression bit, Upcut at the bottom and Downcut at the top!

The disadvantage is that all the chips meet somewhere in the middle hence the compression name so make sure there is some way for them to get out. Normally these will have a short Upcut section at the bottom and a longer Downcut section at the top rather than a meet in the middle design as this allows much more flexibility in machining different thicknesses of stock.



What the bit is made of not what you are cutting. A basic rule of thumb is that the bit must be a lot tougher than the material you are cutting but there are a lot of other factors such as rigidity, wear resistance and don’t forget cost.

I did take a course in Metallurgy a long time ago but nowadays the nuances of the metal blend escape me.



High Speed Steel, this is pretty much a generic description for a modern steel blend designed mainly for high-speed tools.


Carbide / Tungsten Carbide

Carbide is a compound of Carbon and a metal. Carbide tools are normally formed using tungsten as the metal. This has a very high wear resistance and so keeps sharp for longer but it is also expensive. Often a tool will be made from HSS with just the cutting surfaces made from Carbide. Tungsten Carbide is harder, stiffer and will wear less than HSS.



A coating can be applied to the bit to enhance mainly to enhance its resistance to wear, reduce friction heat transfer and finish quality.


Nano Blue Coat

“A high performance Nanograin (very small particles) carbide and silicon coating giving 2-3 times better tool life than a micrograin carbide coating.”



A titanium nitride coating to enhance cutting performance and wear. This has a gold colour.



There are a myriad of other options including no coating, the differences between them are beyond my comprehension and best left to materials scientists and professional machinists!


Milling and routing terms

Not really about bits but everything in CNC is related somehow! This may help if you are just starting out!



Mainly for laminated materials this refers to the action of the bit as it cuts causing the top (or bottom) surfaces to separate slightly and results in splinters on the surface. Other materials can do this as well, normally hardwoods, softwoods can have ‘strings’ left on the edges of a cut, which is basically the same.


Climb vs conventional milling

Any router bit will be turning clockwise, that is traditional and small router controllers will only turn the motor in a single direction which is clockwise. In very simple terms the bit is being moved into the stock at a constant speed while rotating clockwise. Each flute will carve out a chip from the stock as shown by the dotted line due to the movement and rotation of the flute as it turns and moves.


Conventional milling

The chip will start off small and get thicker as the bit moves and rotates.


Climb milling

The chip will start out thicker and get smaller end up smaller as the bit moves and rotates.

Climb Milling will normally leave a cleaner finish with less splintering at the top than conventional milling.

As far as I can tell climb milling gets the name as the bit will try and climb out of the stock unless firmly held, but please don’t quote me on that.


Spindle speed

The rotational speed of the bit in Revolutions Per Minute, often just referred to as Speed.


Spindle Power

The power of the spindle motor, measured in Horse Power (HP) or Watts. The ‘standard’ power of the ‘standard’ 775 spindle motor on a 3018 is around 60W, or 0.06Kw, or 0.08HP. (Think more of Hamster Power!)  Larger routers may have more powerful motors, 300W is a common option and many routers have the option to fit much more powerful motors.


Feed Rate

The speed at which the spindle is being moved into or across the stock. The faster you move the bit through the material the quicker it will cut but it will also put more stress on the bit and the machine. If you exceed the federate that your router is capable of for a cut then the stepper motor will skip or lose steps or the spindle motor may stall and your work will be ruined. Often just referred to as Feed


Max Feed

The maximum achievable feed rate for the router. This is normally the feed rate the router is capable of moving the bit without any cutting load, not the rate at which it will cut! For a Grbl based machine, this is held in the settings as $110-112 for the X, Y and Z axis respectively.



How many times the cut is repeated at a slightly greater depth. If you are using a DOC of 1mm to cut to a depth of 5mm you will need 5 passes, each one 1mm lower than the last. You may also see a finishing pass mentioned, this is where the final pass is run with a lower DOC to give a better surface finish.


Feed per Revolution

Calculated value dependant on the Speed (RPM) and Feed. It’s how far the bit moves along the cutting path in a single revolution.



Quite simply as the bit is pushed through the stock it will bend! Smaller diameter bits will bend more than bigger ones, the greater the stickout and the amount of material it is being asked to remove the more it will bend. If the bit bends too much then it will break!

If the bit is bending the quality of the cut and surface it leaves behind will suffer. This is one of the main reasons that tapered bits exist, it leaves a small cutting area for better detail but the shaft increases in diameter reducing deflection.



If a bit rotated perfectly then the runout would be zero. But it won’t be quite square in the holder, the spindle of the motor will not be perfectly mounted and straight so when the bit rotates there will be a bit of a wobble from side to side, this distance is the runout. Small values are good, if it gets too large then the cut will suffer.



The distance the bit is moved sideways between each cut or line. This can be expressed as either an absolute distance or a percentage of the bit diameter depending on your CAM software. 0 would mean that the bit would just retrace the previous cut, anything over the bit diameter or 100% would mean that ridges would be left between each cut.

The greater the stepover the more material will be removed on each cut but at the cost of a lower surface finish.


Stepdown (AKA Depth of Cut)

When cutting the distance the bit is moved down for each pass, the greater the Stepdown the faster a cut will be made as it will take fewer passes but will increase the stresses on the bit and the machine. These are small machines so use small values to start, 1mm is quite massive on these small machines but it depends on what you are doing to what.


Lead in and out

The way the bit is moved into and out of the cut, the options, if any, you have depends on your CAM software. Some CAM software allows a separate spindle speed and feed to be specified for lead in and lead out operations.



Where the router gradually applies the Stepdown as a ramp rather than plunging and then cutting horizontally.



Moving straight down or plunging into the stock. Normally used as a lead in/out method, though it could apply to drilling. This is the most aggressive lead in method. NOTE: Do not use with compression or downcut bits! They move the chips down and so when plunging leaves them with no way to leave the cut and will cause the bit to clog, overheat...!


Spiral and helical

Other lead in methods, one will lower the bit in a spiral ramp, the other will use a helical ramp. These terms can also be used to describe the toolpath used.



What you get when the chips are too fine, basically they stop being recognisable chips and become sawdust. You can reduce this by slowing the RPM and/or increasing the feed rate so that the bit is cutting larger chips.

Cutting too small chips can greatly increase the heat generated by friction between the bit and the stock as the chips are supposed to carry a lot of the heat away. This can be especially important when cutting materials such as plastics with a low melting point where it’s not so much sawdust as the bit looking like the centre of a candyfloss machine due to the material melting and sticking.



What you get when the chips are too large. Called this as the machine is overstressed trying to push the bit it starts to make chattering noises and gives an uneven surface finish.

This can be reduced by increasing the RPM, decreasing the feed rate, possibly decrease the depth of cut. It is advised to only change one at a time and see what happens.


Surface speed (AKA Cutting speed)

This is just the speed that a single flute at the circumference of the bit travels across the surface of the stock. Surface speed is also a measure of the heat generated by friction which can be especially annoying when cutting materials with a low melting point like plastics.


Chip Load (AKA Feed per Tooth)

This is a measure of the thickness of the chip that each flute will carve out of the stock. Chip Load does not depend on the diameter of the bit BUT larger bits can normally handle a larger Chip Load simply due to the fact that the flutes will be larger and the bit more rigid. If the Chip Load is bigger than the size of the flutes you will have problems.


Material Removal Rate (MRR)

This is the rate at which material is removed from the stock. Higher MRR values mean you are going to get rid of the waste material faster.




A Softwood comes (mostly) from evergreen trees ( such as Pine, Fir, Spruce….) A hardwood comes from a deciduous tree (mostly). It’s far more complex than that. But just remember that Balsa, the softest of all woods is actually a Hardwood!!! However the internal structure of the wood is different between Soft and Hard woods. I hope that helps you as much as it helped me!


Janka Scale

There is a test for the physical hardness of a wood called the Janka scale. It measures the hardness by taking a steel ball 11.28mm in diameter and measuring the force needed to push it into the wood to ½ the diameter of the ball. Beware! the force can be measured using different units, pounds-force (lbf), Kilograms-force (kgf) or Newtons. Just make sure if comparing woods that all the measurements use the same units!

Ebony takes 14,300N (3,220lbf), Rosewood takes 7,900N (1,780lbf), White oak 6,000N (1,360lbf), Douglas Fir 2,900 (660lbf), Western White Pine 1,900N (420lbf) Are just a few examples, search for Janka hardness test for more.

Does this mean for example that speeds, feed and DOC shold be roughly halved from Douglas Fir (Janka 2,900) to White Oak (Janka 6,000)? Unfortunately it’s not quite that simple, but at least one of them needs to be reduced!



Acrylic comes in many grades, and types, not just Cast and Extruded but also from Soft to Bullet-Proof!

When engraving or cutting acrylic and any other plastic it is best to get the bit to take as large a chip out of the stock as possible, this carries away the heat caused by the cutting and rubbing of the bit against the acrylic and helps prevent the plastic from melting. Making a larger chip means increasing the feedrate and reducing the spindle speed.


Soft Metals

Aluminium can be alloyed with other metals to change the properties, a quick tot up shows, well I stopped counting when I reached 100 types! Copper, Brass… also have many grades with diffferent properties and hardness. So all speeds and feeds are just guidelines based on a ‘typical’ material.


Hard Metals

Things like Steel, Titanium… are really beoynd the capabilities of these machines so are not covered here.



There are a multitude, Wax, Resin Board, PCB……. Again these are not covered here.


How to select the right bit

This has nothing to do with speeds feeds etc. but is a little more practical before you try and determine what speed and feed to run it at. I can give no answers, just some questions to think about.


What do you have?

A very important consideration, if you don’t have one you can’t use it! OK you could always buy some more!


Bit Size?

What is the width of the smallest detail you are leaving? This will vary if you are using both finishing and roughing passes.

Imagine you are carving letters in relief, the finishing bit diameter must be able to fit in the smallest gap between the letters and into the letters themselves, an A may be 1mm away from other letters but what is the size of the hole you need to make in the top half of the A or the bottom part of an a?

Another thing to consider is internal radii, if you want an internal corner to look square then you are going to need a very small diameter bit, it’s never going to be precise as you cannot cut a square internal angle with a round bit or a vertical surface with a V or tapered bit.


Bit Shape?

Sometimes obvious, if you want a V shaped groove, well use a V bit! It’s sometimes more subtle though. For finishing a 3D carving then a round nose or ball end is a good choice, they are good at finishing smooth curves.


What are you doing?

Seemingly obvious but still has to be thought about. Even if V carving with a V Bit there are still the questions of what V Angle do you want the finished work to be, how deep will the cut be....


The material you are using?

This makes a lot of difference! How hard is it? Trying to cut and engrave Ebony is very different from Pine.


Creating a toolpath.

Once you have selected the bit there are a number of parameters used in setting the speed and feed you want to use relating to the bit you are using. You need to tell your CAM software:

  • Which Bit you are using.
  • Depth of Cut.

There will be others like retract and safe heights, origin……. But these have little to do with the bit.

There are two ways to get perfect results.

  1. Luck!
  2. Repetition and personal experience.

Experiomentation and record keeping are vital, If you are using natural materials like wood then even if you are using the same species each piece will be slightly different, there are a multitude of softwoods and hardwoods each having different hardness and grain.

My method is to start off with small pieces and make test cuts or pieces until you get good results, then scale it up if needed. I also record the results (only the good ones) to give a starting point for future projects.



Not just the spindle speed and feed rate but things like stepdown and stepover are also very important and included here.

The routers I am using are what I would call Hobby routers, having said that they can and will turn out good results and something like the 6050 and others are moving out of the ‘hobby’ category.


How your router model affects speeds and feeds

The rule of thumb – You get what you pay for – applies here, faster more powerful, more rigid and larger all add to the cost.


Spindle Motor

This is going to have a number of characteristics, the most important ones being:


This determines how much work you can ask the motor to do while maintaining the speed. Higher power motors can cut bigger taller chips than lower powered ones.

Speed range

A Spindle motor will have a maximum RPM it can achieve, also a minimum RPM that it can operate at without risk of stalling. Higher RPMs mean that the bit can be moved further into the stock for each rotation keeping the chipload the same.


Movement rates and power

This is down to the power of the stepper motors and the gearing of the leadscrews or belts. The more powerful the stepper motors the faster the bit can be moved through the material. NOTE: The maximum travel rates are normally based on no load movements, the maximum cutting federate will normally be lower.  


Difficult to measure but does affect the accuracy of a cut and the surface finish. If the bit is able to deflect from it’s intended path the results will not be as good as a more rigid router.


Adding an expansion kit may affect rigidity of your router slightly but apart from that should have no effect at all on the speeds and feeds.


At the moment Speeds and feeds are provided for ‘3018’ routers, unmodified. All these models use a standard 775 spindle motor and Nema17 stepper motors with similar gearing. While the speeds and feeds are for the 3018 PRO the values should form a basis for the other models.

  • SainSmart Genmitsu 3018 PRO, and with the 3040 expansion kit fitted
  • SainSmart Genmitsu 3018 PROVer V1, and with the 3040 expansion kit fitted
  • SainSmart Genmitsu 3018 PROVer V2
  • SainSmart Genmitsu 4040 PRO


I am limiting this guide to SainSmart Genmitsu bits, what I would call affordable bits. My router was not expensive so I am not really interested in using ‘professional’ bits at more than £50 each, even if I could fit them into my ER11 collet holder. (Actually I am not really interested at £25 each, that was just a random figure, and I definitely do not have a poster of a 6 flute 25cm long end mill using internal coolant on my bedroom wall!)


Setting up your router

What does this have to do with a bit? There are settings in Grbl for Spindle motor speed, travel rates and acceleration. While these are not linked to a specific bit they do affect how the bit will work.

Grbl has settings for Maximum ($30) and minimum ($31) spindle motor speeds. If the Sxxx value in your gcode is outside their range the $30 or $31 value will be used instead.

Speed and feed suggestions are for a standard 3018 with the 775 spindle motor. They are based on a maximum spindle speed of 9,000 RPM and a minimum spindle speed of 1,500RPM ($30=9000 and $31=1500) These must be set accordingly.


Accompanying files

NOTE: Facebook has a problem, it will not allow compressed files (.zip, .gz, ......) to be uploaded to the Files section of any group, but it bases this decision solely on the file extension, not the contents. It is easy to bypass this by changing the file extension before uploading, I use .zip files, and rename them to .zipp before uploading. This means that after downloading you will have to reverse this by renaming any xx.zipp file to, windows will issue warnings that you are probably going to make the file unusable, just ignore it and rename anyway. Then you can open and extract the files as you wish. The actual files are in the Tool Databases section.

Older Post Newer Post


Leave a comment

Please note, comments must be approved before they are published