Speeds and Feeds

We know this can be a daunting task with the vast variety of cutters but it doesn't have to be!

Picking the right RPM for your Spindle

To make it simple our starting points are-

Under ⅛ DIA. tools 20000 RPM or greater

⅛ to ¼ DIA. tools 18000 RPM

⅜ to ¾ DIA. tools 16000 RPM

For surfacing/Slabbing/Spoiler board cutters pay attention to the RPM on the tool these tools are balanced to run at specific max rpms.

Coming up with a Feed rate

Next we are going to have to figure out what our feed rate is at those RPMS. We will need to take the chip loads from this chart in order to calculate that number. Here is a chart of the recommended chip loads. The chip loads are in a range so we always recommend starting in the middle and making adjustments based on the result.

Material1/8"1/4"3/8"1/2" and Higher
Hard Wood .003-.005 .009-.011 .015-.018 .019-.021
Soft Wood/Plywood .004-.006 .011-.013 .017-.020 .021-.023
MDF/Particle Board .004-.007 .013-.016 .020-.023 .025-.027
High Pressure Laminate .003-.005 .009-.012 .015-.018 .023-.025
Phenolic   .004-.006 .006-.008 .010-.012
Hard Plastic .002-.004 .006-.009 .008-.010 .010-.012
Soft Plastic .003-.006 .007-.010 .010-.012 .012-.016
Solid Surface .002-.004 .006-.009 .008-.010 .010-.012
Acrylic .003-.005 .008-.010 .010-.012 .012-.015
Aluminum .003-.004 .005-.007 .006-.008 .008-.010

For tools under ⅛ diameter divide the chip load by ½ and increase based on results.

The formula for calculating feed rate is RPM X CHIPLOAD X #FLUTES

For example lets take the Vortex Tool #1230 Upcut finishing tool and calculate the speed and feed for Hardwood. This tool has a ¼ in Cutting DIA. with 2 flutes with those parameter based on the information above we know we are going to start at 18000 RPM and use a .010 chip load for hardwoods. 18000x.010x2=360IPM

IPMmeans inches per minute


(These are starting points so you can increase the depth or back off depending on the results)

Max Axial Depth of cut for ¼, ⅜ and ½ DIA Tools are 2X DIA.

Max Axial Depth of cut for under ¼ DIA tools is 1 to 1 (for example a ⅛ DIA tool should only cut ⅛ deep)


(These are starting points so you can increase the depth or back off depending on the results)

With lighter duty CNC and hobby CNC machines we recommend keeping the tool diameters to ⅜ and under. One of the biggest differences between industrial CNC and lighter duty/hobby CNC is the spindle HP and machine rigidity.

We recommend a starting depth of cut to be 20% of the cutter diameter. Also starting at feed rates that are around 50 IPM at an RPM of 18000. We will be adding more specific information very soon for speed and feed recommendations for lighter duty CNC machines so stay tuned.

Depths of cuts with compression cutters

Compression cutters are a slight exception to this rule as they have an Upcut length. The Upcut length is the tip of the tool opposite to the spindle (what engages onto the material first).

The Upcut length is important because the tool needs to be engaged slightly passed the Upcut length minimum of .063 (1/16) of an inch passed.

For example if we have our Vortex #3420 calls out a .5 Upcut length. The tool should be programmed to cut minimum of .563 at once pass. This will ensure the upper portion of the tool which is the down cut is engaged actually achieving an Upcut tool closer to the bottom of the material and a Downcut towards the top of the material to achieve a nice top and bottom edge on the wood.

Feeding the the Tool into the material

Plunge the material at a 45 DEG angle over 2-4 inches if possible at ⅓ of the calculated feed rate.

When Taking a Finishing Pass With a Finishing Cutter

On finishing passes always take minimum of chip load on radial depth of cut otherwise you are just wearing the tool out.

Radial depth is the depth is the engagement of the side flute of the tool into the material.

For example for a ¼ inch dia. tool in hardwood leave .010 to remove with the tool to allow the cutting flute to engage on the wood that allows for the right size chip that will push the heat of the cut into the cheap allowing for a longer lasting tool.

Ballnose/Tapered Ballnose Tools

The speed and feeds of ballnose type tools are the same as regular tools. The main difference is to make sure to calculate the speed and feed with the diameter of the tool that is being engaged.

See diagram below-

The engagement diameter shown below is roughly .13 of an inch which would mean to use the recommended RPM of that diameter tool.

Please note that this Diameter does change the deeper the tool is programmed to cut.