Which End Mills Should be in the Tool Library?

This is a tricky question to answer as setting up tools takes time. However, the more you add, the better the results you will get from CAM Assist across a wider range of parts: it’s a matter of getting the right balance.

Following are some guidelines to help you decide what balance is right for you.

Guidelines for End mill selection

Tool diameter

A good range of diameters is important in order to handle a range of parts.

It’s recommended you avoid the situation where the next largest tool in your tool library is more than 50% larger than the previous.

For example, if you have a 6 mm tool, 50% larger is 9 mm. However, that’s an uncommon size so you should have an 8 mm tool.

Suggested set of diameters

• Imperial - 1/16 in (0.0625), 3/32 in (0.09375), 1/8 in (0.125), 3/16 in (0.1875), 1/4 in (0.25), 5/16 in (0.3125), 3/8 in (0.375 in), 5/8 in (0.625), 3/4 in (0.75)

• Metric: 2 mm. 3 mm, 4 mm, 6 mm, 8 mm, 10 mm, 12 mm, 16 mm, 20 mm.

Tool Usable Length

It is a good idea to make sure that, at each diameter, you have a tool capable of machining more than 5 times the tool diameter (for example, a ‘Shoulder length’ of at least 5xD).

Tool catalogs often call these “long reach” tools or “long neck” tools. Unfortunately, part designers sometimes work to this 5xD rule when choosing corner radii, failing to recognize that machining a corner with a size-for-size tool is undesirable. Therefore to drop down a tool size, you often require a tool with 6 or even 7xD reach.

Since such long tools are impractical for everyday use, it’s recommended that, for each diameter, you have a general purpose “short” tool, and a rainy day “long” tool. Since the feeds and speeds of the short tool will typically be faster, CAM Assist will choose the short tool wherever possible and the long tool only when required, or when the total number of tools used can be reduced.

Adding longer tools is all the more important if your short tools do not cover every diameter, as described above.

Operations

The above applies to all Fusion 360 operations. CAM Assist works best if you have a range of Roughing, Wall finishing, Flat finishing, and Helical boring tools. These can be the same tools as each other, or a different set of tools for each operation.

Corner Radii

Often, it is difficult to access 3D features with a ball nose tool. If you add Bull nose endmills with corner radii, CAM Assist will also use these tools for 3D toolpaths, for example to create fillets.

In fact, it’s recommended that most of your tools have a small corner radius, 0.2 mm or 0.005 in (5 thou). Any larger than this and the tool will not be used for machining square pockets, which reduces the versatility of the tool.

Quantity of End mills

You can add as many end mills as you like to your tool library. However, a minimum of 10 is essential for good results on a range of simple parts; diminishing returns occur after about 30 tools.

If you follow the guidance above, you should find that you are able to machine most common geometries with less than 30 End mills.

Next step

This section of the Tooling Guide has concentrated on End mills. For details of what else to include, see Which Other Tools Should be in the Tool Library?