CNC Guide (Part 2): How Changing Features Can Mitigate Manufacturability (.PDF Download)

Oct. 27, 2017
CNC Guide (Part 2): How Changing Features Can Mitigate Manufacturability (.PDF Download)

A part’s features sometimes make it more difficult to manufacture, or can increase cost and time. Understanding what affects the difficulty, time consumed, and/or cost of a part that needs to be machined is important. The following presents tips on designing parts for manufacturability with vertical milling machines, horizontal milling machines, and lathes. For more information, check out Part 1 of this guide.

Interior Fillets

When using a CNC vertical or horizontal milling machine, all interior vertical walls must have a radius. That’s because a round tool, spinning at high RPMs, is used to remove the material. Designs must take into account areas where radii will occur due to this limitation.

Inside Corner Fillets

For inside corner radii, it may be better to use a non-standard radius. This is because end mills need clearance to turn and continue milling when tracing the internal corner. If a part features a 0.25-in. interior radius, the standard end mill would need to hammer the corner, come to a complete stop, pivot 90 degrees, and then resume cutting. Doing this slows down machining speed, which adds costs and causes vibration. By adding 0.02 in. (0.508 mm) to 0.05 (1.27 mm) in. to internal radii, the cutter will be able to turn slightly without coming to a complete stop. This will not only reduce cost, but also improve CNC parts.

The larger the radius, the lower the cost. The reason for that is a larger tool can be used, which means more material can be removed with each cut, thus reducing the time to machine the part. For example, a tool with a 0.125-in. diameter (0.063-in. radius) would take approximately 1.5 times longer to perform the task than using a 0.187-in. diameter tool, and approximately two times longer than a 0.250-in. diameter tool.

Even though small-radius tools (down to a 0.015-in. radius) are available, sometimes the depth that the tool needs to go into the material makes it impossible to cut because the tool is not manufactured. If the tool is manufactured, the cost will increase significantly due to the fact that only small cuts can be made, which extends the manufacturing time.

When the depth of cut becomes greater than two times the diameter of the cutting tool, then the feed rate of the tool will need to be slowed down, leading to increased cycle time and costs. For every doubling of the depth of cut, the feed rate is more than halved, which more than doubles the time to cut the feature. The max cut depth to tool diameter ratio is six times; beyond that, special tooling will need to be ordered. For example, if a 0.125-in diameter tool is used, then the max cut depth would be 0.750 in. before having to use a custom tool.

Voice your opinion!

To join the conversation, and become an exclusive member of Machine Design, create an account today!