2019cnc4-5

60 www.CNC-West.com CNC WEST April/May 2019 CAD/CAM/CNC Perspective By: Tim Paul Tim.Paul@Autodesk.com 3D Toolpaths, tying it all together… In the last two issues, I explored the details of 3D machining toolpaths. I covered some of the funda- mentals that changed my 3D machining game, including tessellated surfaces, boundary conditions, the effects of smoothing on point distribution, knowing your priorities, and the way I break surface geometry into different categories based on how toolpaths interact with those geometries. In this issue we will wrap up the 3D toolpath discussion. I often overuse the phrase “the devil is in the details” because I can’t think of an industry that it applies to more, and 3D machining is especially full of important details. This article will focus on some of the finishing details in tooling outside of the CAM software that play an equally important role in producing consistently high quality finishes on 3D surfaces. Tooling: When finish machining 3D surfaces I generally fol- low these steps: 1: Optimize my setup to create the best cutting con- ditions possible. 2: Select the proper tool for the material and geom- etry being cut. 3: Select appropriate roughing processes before finishing. Optimize setup to create the best cutting condi- tions possible: Ball nose end mills are ideal for machining 3D surfaces. However, when machining flat or shallow surfaces that are perpendicular to the tool a zero SFM (Surface Feed per Minute) condition occurs. A zero SMF condition means that the surface speed of the cutting edge of the tool get closer and closer to zero as it gets closer and closer to the center of the tool when it is effectively zero. A zero SFM condition does two main things. 1: It creates incon- sistent surface finishes on shallow or flat surfaces when the center of the tool is engaged with the surface. The flat or shallow surfaces will often have smear marks where the tool essentially pushed the material out of the way instead of cutting it . These marks are often dull and occur on shallow areas. 2: Tool life is reduced when cutting in a zero SFM con- dition. The part material dictates what mechanism will reduce the life of the tool. Soft materials such as Aluminum will weld material to the cutting edge while harder materials will break down the cutting edges. Whenever possible, I try aligning the part in the machine to reduce or eliminate the possibility of zero SFM conditions. One of the many benefits of multi-axis machines is their ability to easily align the surfaces being machined to optimize the cut- ting conditions. One of the many benefits of 5-axis simultaneous machining is the ability to specify the tool vector or specific engagement of the tool. Often a simple 3+2 positioning move will create an ideal cutting condition for a variety of surfaces. Angling a surface to be 15 degrees off perpendicu- larity to the spindle creates a much better cutting condition. Whether you can angle the surface to eliminate the zero SFM condition or not, it’s important to opti- mize the surface speed for the conditions. There are plenty of good references for the specifics of calculating the Effective Cutting Diameter and ad- justed velocity for a ball mill while considering the incline angle/tilt and the ADOC (Axial Depth Of Cut), so I’ll skip the formulas and diagrams in this arti- cle. Many cutting companies have detailed this, one quick source can be found in the tech area of the Helical Tools website. The core of what you need to account for, unless you are cutting at full radi- us of the ball, is the ECD (Effective Cutting Diam- eter). Examples: At zero degrees of tilt, a ¼” ball end mill cutting an ADOC (Axial Depth Of Cut) of .010” has an ECD of .098”. The same ¼” tool at the same .010” ADOC with a 15 degree forward tilt has an ECD of .154”. Once you’ve calculated your ECD you need to then calculate an adjusted RPM to match an ideal cutting speed to the EDC. You will likely need to increase your RPM, often an increase to the maximum spindle RPM is needed to get as close to the calculated ideal SFM as pos- sible. I think of it as simple as calculating the SFM to the size of the tool that is actually cutting. Select the proper tool for the material and the ge- ometry being cut: Appropriate tooling is one of the more important variables to control when machining consistent 3D surfaces. There is a lot more to tooling than just the cutting tool. I think of tooling as the cutting tool, tool holder, work holding, and even small auxiliary details such as the coolant. Many tooling basics apply to selecting an appropri- ate tool for machining 3D surfaces the same way