This page is for a reference and is from my own research into calculating tool speeds and feed rates for different materials. Also I will attempt to explanation the different tooling and what jobs and materials they are used for.
preparing for the cut
Before making the cut we have to first prepare the path within our CAD/CAM package with a few additional settings other than our usual feed rate. To do this we have to decide on what type of pass we are going to make.
Depending on the project it may be beneficial to machine the project with two passes. The first pass is called a roughing pass which aims to remove as much unwanted material as quickly as possible. The second pass is called a detailing pass, smoothing the edges and adding the intricate detail.
To remove as much material in the shortest time possible one or a combination of the following may be used:
- A larger bit to move as much of the material as possible.
- Increasing the load on the tool to remove more of the material at any one time.
A larger bit such as a large straight flute to create a large pocket can be used in the first pass to remove large amounts of material. Additional passes can be made with progressively smaller bits progressing us to a point where we can swap to a smaller bit for the more intricate parts of the project.
Increasing the load on the tool means removing more material by cutting further and deeper into the stock. This can be done by increasing the depth on each decent on the Z axis and / or increasing the step-over value for removing material on the X and Y axis.
For roughing a common step-over setting is around 35 – 40 % of the bits diameter being used.
The cutting depth on the other hand will depend on the ability of the CNC machine and the material being used. In the case of using the MDF with a 6mm solid carbide cutter, a common approach seems to be to use 2mm steps and a very fast feed rate. You shouldn’t get fine powder dust from the MDF but more like wood shavings. If you go too slowly the bit will gum up, burn out and blunt quickly due to the build up of friction. When a tool makes an unhappy noise it means that either the RPM or feed rate are wrong.
A finishing pass is the reverse, removing smaller amounts of material adding detail and smoothing the surface. To do this we can use a combination of a smaller bit, reduce the depth of cutting and decrease the step over by about 3-5% width of the bit. We will be running the tool faster with less load rather than slower with more.
What is step over?
A tool can be configured to make several adjacent cuts rather than passing the full diameter of the bit for the next cut. For example, to cut a 12 mm width pocket with a 6mm bit we can make 2 passes to remove the material. Though the fastest option this has two disadvantages. Firstly a high load on will be applied to the bit so a slower speed rate will be needed and / or a decrease in the depth and, secondly a ridge of unwanted material, called a scallop, will remain between these two cuts leaving a rough texture. By using step-over we increase the amount of passes but still maintain or increase the feed rate. In our example if we change the step over from 100% to 50% then we will cut the diameter of the bit (6mm) on the first pass then 50% (3mm) of new material on the second and finally another 50%, completing our 12mm width pocket in 3 passes rather than two. This results in a smaller scallop left. The less material removed in each step the better the finish (but the longer it takes to complete).
Router / Spindal Speeds
To calculate the correct speed rate we need to know the speed of the tool being used. Rather than a spindle I use the cheaper alternative, a hand trimmer (also known as a mini router) the model of which is a Katsu 101748 which is apparently mechanical similar if not identical to the more expensive Makita RT0700.
The speeds of the router is defined in the user manual. I have checked both Makita and Katsu and they both seem to have the same RPM for each of the numbered speed settings on the dial. I have included the table below as reference.
Calculating Feed Rate
To calculate feed rate and tool speed for cutting the optimum chipload is one of the most important parameters of all to get right. Chipload is the size of the material that is removed by each cutting edge (flute) in a single revolution of the tool bit. If the chips are too small i.e. we create dust then heat is generated, blunting and burning out the tool.
The formula to calculate the feed rate is:
f = n x cpt x rpm
|n||number of flutes, the cutting edges|
|cpt||chip per tooth, the chipload or material removed by each revolution of the tool bit measured in mm per tooth|
|rpm||revolutions per minute of the tool bit|
‘Ball Park’ values for chip load
|Bit Diameter||Hard Woods||Softwood / Plywood||MDF / Particle Board||Soft Plastics||Hard Plastics||Aluminium|
|3mm||0.08 – 0.13||0.1 – 0.15||0.1 – 0.18||0.1 – 0.15||0.15 – 0.2||0.05 – 0.1|
|6mm||0.23 – 0.28||0.28 – 0.33||0.33 – 0.41||0.2 – 0.3||0.25 – 0.3||0.08 – 0.15|
|10mm||0.38 – 0.46||0.43 – 0.51||0.51 – 0.58||0.2 – 0.3||0.25 – 0.3||0.1 – 0.2|
|12mm and over||0.48 – 0.53||0.53 – 0.58||0.64 0.69||0.25 – 0.36||0.3 – 0.41||0.2 – 0.25|