Choosing Tools

On This Page:

Tool Diameter

When choosing a ball end mill to define a smooth surface, always choose the largest size available. For the same stepover, a larger tool will leave smaller scallops, thus giving a smoother result. For a generally smooth model with some areas of fine detail, a large tool should be used for the overall job and a smaller tool should be used only to clean out detailed areas. This will save time and help extend the life of the tool, avoiding broken tools.

Larger tools cut more cleanly, have larger clearance, and stay sharp longer. The velocity of the cutting edge on a larger tool is higher for the same spindle speed than on a smaller diameter tool because the outer edge is farther away from the center of the tool.

Internal corners will always be rounded regardless of the diameter of the selected tool, but larger diameter tools will obviously create corners with larger filleted radii than small diameter tools. When creating shapes that need to have tight corners, it may be desirable to use as small a diameter endmill as possible. However, it is generally best practice to first clear away all material with a larger diameter tool and then come in for the final finish pass with a small diameter tool.

Tool Length

Small diameter tools are less rigid and more prone to vibration than larger diameter tools. In turn, means that small diameter tools cannot be as long or extend as far out of the holder. When extended out far from the tool holder these tools are more prone to breaking and are not as well suited to creating a nice surface finish as those that are larger in diameter. In general, it is best practice to always use as large of a diameter as the geometry will allow, this will extend tool life.

End Geometry

End mills come in a variety of shapes. The most common are flat end mills and ball end mills. Flat end mills will cut flat areas with no scallops. However, they leave a terrace-like scallop on non-flat surfaces. Ball end mills will leave smaller scallops for the same stepover value on sloped surfaces, but they will also leave scallops on flat areas.

Parts can be machined with a combination of tools with both flat- and ball-end geometry. If only one tool will be used for all surfaces of different slope characteristics, ball end geometry will give a more consistent overall feel and smooth result. To obtain large smooth terrain surfaces, it is generally recommended to use a large diameter ball end mill.

Flute Geometry

While the number, direction, and type of flutes that a cutting tool has can vary widely, the tools most commonly used at the GSD have two flutes and are up-cut spirals. This flute geometry evacuates chips from the cut area efficiently (upwards) and the number of flutes does a relatively good job of removing a significant amount of material and producing an acceptable finish quality.

Some projects may benefit from other types of flute geometry. For example, contour cutting plywood sheets can benefit from compression spirals for through-cuts and down-cut spirals for other operations. Compression spirals have flutes that go in both directions, up from the bottom and down from the top. This action maintains a good finish on both the top and bottom of the sheet of material. These tools are designed to cut through sheet material in one pass, without the use of depth cuts. Down-cut spinrals push the material against the CNC machine table as it cuts, rather than lift it, helping to both hold the material to the table and also reducing any material blow-out on the top of the part. As down-cut flutes do force the cut material chips downwards into the cut, there is an added risk of fire in some applications of this tool.

Straight flute geometry does not lift material up as it cuts, rather it just pushes it backwards. This action makes this flute geometry less suitable to cutting recessed areas in parts where the removal of material upwards is necessary.

The Flute Length of a tool is the length of the tool that is designed to cut. Although the spiral geometry of the tool may be 2" long, with closer inspection you may likely find that only 1.5" is shaped and sharpened to the point where it is able to actually cut. It is important that one never exceeds the cutting length of the tool with any one cut depth or stepdown, as this would cause non-cutting portions of the tool to collide with the material. Such a collision will damage the tool, will damage the material being cut, and can even cause fires or other hazardous conditions.

Stepover

Stepover is the distance the tool moves between subsequent lateral (XY) passes.

It is the stepover value (in combination with tool diameter) that will determine whether the model has a smooth finish and the visibility of tooling marks on the machined surface. This parameter will also impact cutting time directly. Surfaces machined with a smaller stepover will take longer to cut than those with a larger stepover. If the stepover exceeds the diameter of the tool, portions of uncut material will remain between consecutive passes. This can either be desirable, for making highly-textured surfaces, or a problem.