There are many components to the successful implementation of high speed machining. High speed spindles, powerful CNCs, specially designed cutting tools as well as finely tuned process knowledge are all important to shops seeking to master this productive milling technique. These elements have been widely discussed over the last few years, and continue to be constructively debated as our industry comes to understand more about the high speed machining process.

Less recognized, however, is how high speed machining impacts the creation of tool path data -- and perhaps more important, how the creation of tool path impacts the milling process as it plays out in fast-forward on the table of a machining center. CAM technology is coming to recognize the nature of this challenge, however, and providing new features well suited for the high speed machining environment. Here are some of the more significant capabilities to look for in an NC programming system if you are thinking about speeding up both your milling and programming process.

The Challenge

High speed machining often includes machines and controllers that can operate at 25,000 rpm and upwards of 200 ipm. Typically, the NC programmer using this technology will take a smaller cut than one would with conventional machining, but do it much faster than conventional machining. Thus the volume of each chip per tooth is reduced, but that is more than made up for in the speed of the cut.

With high speed machining, keeping the material removal rates as constant as possible is very important. However, complex 3D shapes with floors, walls, valleys and other sloping shapes make this difficult. Sharp corners or sharp changes in tool direction can lead to gouging, tool damage or even spindle damage, and should be avoided if possible.

With the high speeds and feeds, tools are all the more susceptible to damage. Additionally, many tools on high speed machines have reliefs cut either on the sides or directly through them to allow for high pressure coolant or compressed air to evacuate all chips from the workpiece. These coolant cuts will obviously weaken the cutting tool somewhat.

All of these factors combine to place a higher emphasis on how well the tool path is created in the first place. As such, shops should take a second look at their CAM technology in the context of this more demanding cutting process.

General Features

What should they look for? First of all, due to the tighter stepovers typically used in high speed machining, and the desire to reduce hand finishing, a high precision mathematical workpiece model is required. Some packages use different algorithms to tessellate (facet) surfaces depending on which command one happens to be in. This leads to surfaces with different facets used for cutting different program styles, slightly different outputs and redundant calculations. We believe that one high precision polyhedral mesh should be used for all NC operations. This allows for easy creation of a job planner, where many different cuts are set up at one time.

It should go without saying that the model and NC tool path need to be gouge free. With conventional milling, a machine operator often can catch a gouge and stop the program before significant damage is done to the tool. With high speed machining, counting on the operator to catch these gouges becomes much more difficult.

Roughing

The roughing operation takes on more importance in high speed machining than it does in conventional machining. Roughing functionality must leave a more uniform amount of stock for pre-finishing and finishing than it does in conventional machining. As Dr. Josef Koch, director of development at Open Mind Software Technologies, puts it: "High speed machining changes the CAM strategies. More effort has to be devoted to roughing the model more exactly . . . the term pre-finishing takes on more importance."

The common method for roughing is to cut successive levels in the "Z" direction. These cuts will follow the high speed machining theory of a smaller step-down than conventional milling in order to keep the chip-per-tooth value down. To accomplish the uniform stock allowance when roughing in this manner, it is important for the CAM software to compute its Z-level passes based on the proper corner geometry of the cutter being used. That requires a 3D offset for stock allowance if you are using anything other than a flat bottomed cutter for roughing. In terms of the stock left for finishing, the difference between a 2D and 3D offset can be quite dramatic.

Pencil Milling

To clean out corners for semi-finishing operations, the typical method in the past was to pick two surfaces that form a corner and drive a tool along their intersection. This method worked well enough with small or simple parts, or on more complicated parts if there was plenty of time for programming. But because of the time required to manually pick and cut all of the corners for different sized tools, many people choose to forego that step, thereby creating a dangerous condition for high speed machining.

Pencil milling uses an algorithm that finds all of the corners and valleys of a part left over from a previous larger cutter, and automatically drives a tool along those corners. The software allows the user to mill these corners with smaller and smaller tools until the tool radius matches the radius of the 3D corner or valley. Ideally, the software is tracing corners of multiple surfaces in an optimized fashion to reduce retracts.

For example, you have a mold with some walls and a floor in it, and these walls have fillets on the bottom with radii of 1/4 and 1/2 inch. You first cut the model with a 2-inch ball mill, thus leaving a 1-inch radius in those corners. Pencil milling would know of the material left in the corner, and automatically drive the next tool, say a 1-inch ball mill, in the appropriate corners. This would clean up corners with a 1/2-inch radius, but not the corners with a 1/4-inch radius. Then when a 1/2-inch ball mill is selected, the software would drive the smaller tool along the 1/4-inch radius, but it would not bother to recut the 1/2-inch radius corners because that would be wasted motion indeed.

This kind of functionality is particularly important for high speed machining because of the desire to maintain a relatively constant chip removal rate. Without pencil milling, when finishing these parts with walls and floors, the tool would be removing a considerably larger volume of material when it reaches the corners. With pencil milling, the corners are already relieved, causing less tool deflection and noise when cutting the corner. This is true whether machining in a downhill or uphill fashion.

The software should allow the user to choose climb or conventional milling, with climb cutting generally being the best choice for high speed machining. Additionally, the software should be able to go downhill to vertical corners, instead of uphill.

Because pencil milling can clean out stock in corners, where the stock will typically be heaviest, pencil milling is often performed before various 3D finishing methods are run. The machine operator or NC programmer will typically reduce the feed rate of a pencil cut operation due to the increased material removal rate.

Rest Milling

Rest (as in "rest of material") milling is a close sibling to pencil milling, but can do double duty as a finishing operation. Using an algorithm similar to pencil milling, rest milling can find all the areas of a 3D part that were not cut based on one tool size, and cut only those areas with a smaller tool. Rest milling differs from pencil milling in that it cuts the whole area left over from the larger tool whereas pencil milling drives the tool strictly in the corner.

An important option for high speed machining is the ability to compute rest material cuts that are normal or parallel to the cut area. The normal option will raster cut back and forth in the rest area whereas the parallel option will follow the flow of the rest area. People who use high speed machining will typically apply the parallel option, which reduces the number of stepovers from hundreds to just a few, thus making the machining process more efficient. Moreover, as Dr. Koch explains: "By computing a pocket from outside to inside, always in a climb cutting mode, and with the stepover done on the surface, it creates a better finish."

Controlling The Cusp

When cutting complex 3D shapes, the ability to compute the stepover for NC finish passes based on a scallop height versus using a constant stepover has been around in different CAM software packages in one form or another for some years now. The advantage of using this functionality in the past was a consistent surface finish. Typically, less stoning and other hand finishing tasks would be required.

Programming to a user-defined cusp has still another benefit in high speed machining. By dynamically changing the stepover based on NC finish passes, the software is helping to keep the chip removal rate at a constant. This keeps the cutting forces on the cutter to more of a constant, thus keeping any unwanted cutter dynamics to a minimum.

No matter how good the look-ahead feature is implemented in a high speed machining controller, it still does not know what the stepovers are on a 3D part. The look-ahead really only knows about the removal along the tool path and its corners. Look-ahead does not know what the stepovers of a 3D finishing pass are, and does not know the volume of material being removed.

How cutting to a scallop works is that internally the software computes the sloping portions of the 3D shape. The software can then adjust the stepover required to maintain a constant scallop height based on tool size and geometry. Typically, this means the steeper the slope, the tighter the stepover required for a finishing operation. Naturally the user gains the additional benefit of a smooth, consistent finish across the whole model.

Finishing Strategies

The functions for finishing a 3D model must be flexible to allow the operator to tailor the tool path to the part. Some different 3D finishing programs use curve geometry to define a swept tool path as opposed to straight paths. Some systems allow for straight cuts as well as offset, normal, ruled and flow. The CAM operator can choose the best 3D finishing operation based on the shape of the part.

Due to the complexity of 3D geometry, the finishing operation of "blasting" parallel plane cuts on a whole model is no longer sufficient for finishing. These cuts really do not follow geometry in a normal or parallel fashion, and can have detrimental effects on certain corners and walls. This is why many people use rest milling as a finishing operation as previously mentioned.

While cutting with a zigzag pattern is predominantly used with conventional machining, many people choose to use a box or one-way cut with high speed machining. This is because of the time wasted when the NC machine has to immediately stop (by ramping down the speed) due to jerk limitations of the machine and then step over. Additionally, many people will choose to cut in a one-way fashion to maintain climb cutting strategies.

Likewise, other strategies currently favored by CAM operators for conventional milling need to be adjusted for high speed machining. The user needs to be more concerned with his tool and how the tool motion can be controlled in complex 3D geometry. More care is taken when roughing to maintain even chip removals during finishing, and different finishing options are needed to control tool motion.

Mastery of these techniques is not difficult, but it does require programmers to adjust their thinking to the demands of the high speed machining process. And it will certainly help to make sure they have a programming tool -- in the form of an up-to-date CAM system -- that is up to the job. 



http://www.mmsonline.com/articles/119605.html