CNC router bits and carbide cutting tools with tutorials and technical guides

  • Your shopping cart is empty!

First Steps for Machining Wood with Microtools

Before you run the first piece of code and start making chips, there are a few basic practices you should employ to help you get off to a good start. These may seem a bit fiddly at first, but they will help you achieve more reliable cutting, higher feed rates, better cuts and fewer broken bits.

Preparing Your Spindle / Router

To get started:

  1. Clean the spindle bore, collet and nut with ColletCare or a similar cleaner / lubricant ( COLLET CLEANING ). - It is essential that the collet seat into the spindle bore with minimal interference or resistance. Keeping this area clean, lubricated and free from debris will also help minimize runout (aka TIR , "The Bit Killer"). DO NOT lubricate the collet bore as this may cause the bit to slip under heavy load.

  2. Periodically check the runout of the collet you are using (COLLET RUNOUT). - There are a lot of very good technical reasons why you need to minimize runout in your spindle (or router), but they all boil down to the fact that getting control of how much your bit is wobbling results in lower bit breakage, more precise cuts, better fitting inlays and reduced wear and tear on your spindle bearings. More will be said about the importance of measuring and correcting TIR in a later tutorial.

  3. Use "air cuts" to check your code before committing to a cut (you don't even have to have a tool loaded). - Find problems with your tool path, clamp placement, mystery plunges or errant tool paths that land outside your part before you ruin that lovely, and expensive piece of rosewood.

  4. Make sure the spindle turns ON when you start your code. - I know, this sounds obvious, if not a little silly but, sooner or later, we all make this mistake and it can be costly.

  5. Make sure the spindle is rotating in the proper direction when it first spins up. - The vast majority of cutting tools that you will use will be right-hand-cutting (RHC) bits. That means that the spindle should be spinning CLOCKWISE as viewed from the top. An easy way to check this is to look at the spindle nut when the motor first starts turning. The side facing you should be rotating from RIGHT to LEFT.

  6. Mount the nut and collet onto the spindle. - If you are using ER style collets, or our high precision router collets, make sure that the collet is properly snapped into the nut ( ER COLLETS) .

  7. Load the cutter into the collet and tighten the nut to the recommended torque ( TORQUE TABLE). - If you are using cutters fitted with depth setting rings ( DEPTH RINGS ), make sure the ring is pressed firmly against the collet face while you are tightening the nut. If you are using bits without depth rings, insert the bit into the collet as deep as possible leaving a minimum of the smooth shank visible while NOT bottoming the shank in the spindle bore.

Zeroing Microtools

Zero the tool to the top surface of the material you intend to cut (or to whatever height your code considers Z=0). - When cutting with microtools it is generally NOT recommended to use a touch-off plate or to bring the tip down on a piece of paper that you are sliding back and forth to feel a "snag". Both techniques may well result in a broken tool. A more reliable, and repeatable method is to:

  1. turn on the spindle

  2. lower the spindle until the tip of the tool is just above the surface

  3. continuing lowering the spindle in 0.001" (0.025mm) increments while closely watching the tip of the tool (a magnifying glass or jeweler's loop are very useful here).

  4. when you see the tip lightly cut into the surface, stop lowering.

  5. lift spindle one 0 001" (0 025mm) increment and set this height as Z=0

  6. lift the spindle to a safe height.

You are ready to rock.

If you are using very small microtools where it is difficult to tell when the tip first touches the material surface, read our Advanced Z Zero Technique

Rules of Thumb

The most frequent question(s) we are asked has to do with selecting the best feed and speed to use when using one of our tools on a particular material. In many instances the material you are cutting is worth far more than the cutter you are using, not to mention the amount of time you might waste if the wrong cutting parameters are used. For that reason, among others, we always try to take as much time as necessary to help you set up your parameters to get you off to a safe start. Over the past year we have started sending emails to new customers who purchased our micro-tools, suggesting that they call us for help in setting up their first cuts.

So, to get on with it, the first consideration that needs to be discussed is the concept of chip-load (how big a bite each flute takes per revolution). While a lot more will be said about this in a later tutorial, the main takeaway is that setting the RPM and feed rate to achieve a suitable chip-load is crucial for getting enough shear to achieve clean, smooth cutting and to sink as much heat as possible into the ejected wood chips to preserve the life of the tool. Recognizing that this can get very technical, very quickly, we have worked to come up with some easy to remember "rules of thumb" to get you started without a lot of brain death. These basic rules will be implemented using our Feeds and Speeds calculator ( CALCULATOR ).

Things to remember (or write down and stick to your spindle):

  1. When machining wood (soft and hard) with tools with a cutting diameter of 1/8" (3.18mm) or larger , the chipload should never be less than 0.002" (0.51mm).

  2. When machining wood (soft and hard) with tools with a cutting diameter of 1/8" or smaller , develop as much cutting shear as possible by running at your maximum RPM.

  3. Calculate a safe starting RPM for cutting most hardwoods using a value of 800 - 1,000 surface feet per minute (SFM) in the formula:

    a. RPM = (3.82 X SFM)/(cutter diameter)

  4. 3% is safe for ALL of our tools in wood when cutting 1 tool diameter deep per pass (pass depth)- I will explain this below

Making Chips

The most frequent question(s) we are asked has to do with selecting the best feed and speed to use when using one of our tools on a particular material. In many instances the material you are cutting is worth far more than the cutter you are using, not to mention the amount of time you might waste if the wrong cutting parameters are used. For that reason, among others, we always try to take as much time as necessary to help you set up your parameters to get you off to a safe start. Over the past year we have started sending emails to new customers who purchased our micro-tools, suggesting that they call us for help in setting up their first cuts.

So, to get on with it, the first consideration that needs to be discussed is the concept of chip-load (how big a bite each flute takes per revolution). While a lot more will be said about this in a later tutorial, the main takeaway is that setting the RPM and feed rate to achieve a suitable chip-load is crucial for getting enough shear to achieve clean, smooth cutting and to sink as much heat as possible into the ejected wood chips to preserve the life of the tool. Recognizing that this can get very technical, very quickly, we have worked to come up with some easy to remember "rules of thumb" to get you started without a lot of brain death. These basic rules will be implemented using our Feeds and Speeds calculator ( CALCULATOR ).

Things to remember (or write down and stick to your spindle):

  1. When machining wood (soft and hard) with tools with a cutting diameter of 1/8" (3.18mm) or larger , the chipload should never be less than 0.002" (0.51mm).

  2. When machining wood (soft and hard) with tools with a cutting diameter of 1/8" or smaller , develop as much cutting shear as possible by running at your maximum RPM.

  3. Calculate a safe starting RPM for cutting most hardwoods using a value of 800 - 1,000 surface feet per minute (SFM) in the formula:

    a. RPM = (3.82 X SFM)/(cutter diameter)

  4. 3% is safe for ALL of our tools in wood when cutting 1 tool diameter deep per pass (pass depth)- I will explain this below

To see how these will help you get started, we will first calculate the RPM using a conservative value of 800 SFM for a 1/8" diameter bit (this calculation can be done on the calculator page linked above).

RPM = (3.82 X 800) / (0.125") = 24,448 RPM

We will use 4krpm RPM (since that is the maximum speed of our spindle) to calculate the MINIMUM feed rate (0.002" chipload) we should use for a 2-flute, 1/8" dia. end mill cutting 1/8" deep in hardwood. (remember to press "CALCULATE FEED in the lower left) Note: We are ignoring the effect of runout in the sample calculations below for the sake of simplicity.

3 percent is safe

With these inputs, we see that we should consider 96 inches per minute (IPM) as the absolute MINIMUM feed-rate we should set for this tool at 24KRPM. Anything slower stands a good chance of burning the wood and/or burning / dulling the tool. It might sound pretty fast but, as it turns out, it is not really a reasonable feed-rate for this tool.

After years of testing, we can state, with a high degree of confidence, that a safe starting point for the chip-load for ALL of our tools, cutting 1 diameter deep in WOOD, is 3% of the tool diameter (3% is safe!). What does that mean for our example above? Let's plug in the numbers and see.

3 percent is safe

Quite an improvement. Although a chipload equal to 3% of the tool diameter will get you started, it will not necessarily offer the best cut, highest performance or longest tool life.

Once you are comfortable with these simple (but necessary!) steps, don't be reluctant to experiment with larger, and smaller, chiploads.

Note: If your CNC is not capable of reliably achieving and maintaining the feed-rates derived from the calculator, you can lower the RPM until you reach a feed-rate your machine is comfortable with (even it it means reducing the shear developed by the cutting tool).