Make your own free website on

CADCAM for High Speed Machining


Successfully implementing High Speed Machining (HSM) depends on getting a lot of things right all at the same time. The nature of the process is such that – by definition – once things start to go wrong they go very wrong very quickly.

Some of the critical factors are easily defined: a high-specification machine tool, equipped with a powerful CNC and an accurate spindle; stiff and precisely balanced tool holders; high-performance cutting tools. All of these can be specified quite exactly. Other factors are much more difficult to pin down, and it is often these that cause some attempts to implement HSM fail, even though the physical equipment meets the same specifications as other successful implementations.

The quality and appropriateness of CAD and CAM operations are two such major factors. It is obvious when you think about it that the CADCAM system generates the programs for the CNC, and therefore directly determines many process conditions. However it is very difficult to specify exactly what is required from these functions to obtain good results from HSM.

As Development Director responsible for CAM products at Delcam Plc, a leading international supplier of CADCAM systems for the design and manufacture of complex-shaped products, I get to see plenty of examples of good and bad HSM practice. This paper highlights some of the issues in CAD and CAM that I believe are central to successful HSM.


It may not be immediately obvious that CAD has much direct bearing on High Speed Machining. After all, the CAD model simply defines the shape of the part, and it is up to the CAM operator and the machinist to cut what is provided, isn’t it?

In theory this is true, but in many cases the CAD model may not really define the shape to be machined at all. There are several reasons why a model may not be ideally suited to HSM. Most of these will influence conventional machining as well, but usually the effects will be much less significant.


A major benefit of HSM is the ability to machine parts accurately, with minimal thermal distortion and good surface finish. It’s surprising to see how often the tolerances used to create the part model are coarser than the final machining tolerances.

A potential source of accuracy problems is data exchange. Parts are frequently designed in one CAD system and then transferred to different systems for additional design work and for machining. Each data transfer requires geometry to be converted from one format to another, and some of these conversions involve approximation to some finite tolerance. The effects of these tolerances are cumulative, so it is essential to make sure that they are set to be significantly (at least ten times) smaller than the finish machining tolerance.

Exchange formats like IGES often force systems to convert between different geometric representations. If possible, it is best to rely on the sending system to do any conversions, because it has access to the “master” data. This can be achieved by “flavouring” the IGES in the sending system. Flavouring tells the system which of the many possible entity types should be used in the IGES file. Some systems provide a menu of predefined IGES flavours to work with other popular systems.

One way to minimise conversion problems is to make use of direct interfaces. A direct interface allows one system directly to read the files of another. For example, Delcam’s PowerMILL has direct interfaces for Catia, Pro/Engineer, Unigraphics and other widely used systems.

A data exchange format favoured by some companies because of its simplicity is Stereo lithography (STL) triangles. A number of CAM systems – Delcam’s PowerMILL included – can machine STL files directly. However, the triangles are generated to a tolerance and this can result in visible faceting of the machined surface. In many popular design systems the tolerance used for STL defaults to quite a large value (0.1mm) and is buried within a mass of options where it is easy to overlook. Tightening the machining tolerance on a coarse STL file simply machines each triangular facet more accurately!


Most parts are represented in CAD systems by a patchwork of “trimmed” surfaces – similar to the way clothes are assembled from several complex-shaped pieces of material. The accuracy with which these surfaces meet at their edges can have a critical effect on the quality of toolpaths.

Figure 1 - Trimming Errors

Figure 1 shows in exaggerated form what may happen when a cone is capped with a trimmed plane. The cone is exactly circular, but the planar cap is a polygon that may overlap the top of the cone in some positions. If these overlaps are significant they may result in unexpected spikes in the toolpaths and visible marks on the finished part.


Figure 2 shows a more complex model with badly trimmed surfaces where a number of surfaces meet. This kind of problem is most often the result of using an unsuitable modelling tolerance, but trimming problems can sometimes be introduced by data exchange errors.

Figure 2 - Poorly Trimmed model

Incomplete Models
Many CAD operators have developed shortcuts to keep modelling time to a minimum. An often-used shortcut is to omit fillets from internal corners on the basis that they will be formed directly by a milling cutter of a suitable radius. This approach requires that the tool be driven right into the sharp corner; see Figure 2(a). This temporarily increases the load on the tool by a factor of about 4.5 compared with straight-line cutting conditions.

Figure 3 - Cutting Internal Files

Some CAM systems provide functions to cure this problem, but it is much better to prevent it in the first place by ensuring that the CAD model accurtely represents the shape to be machined. It is best to form internal fillets using a cutter of smaller radius, so that the toolpath can flow smoothly round the corner rather than turning sharply, see Figure 2(b). A tool radius of 70% or less of the fillet radius is suitable, and reduces the cutter load by a factor of about 3 compared with the sharp corner.

Unmachinable Features

Although HSM increases the range of features that can be milled directly, complex parts often include details that must be produced by EDM. The majority of parts also have holes that will simply be drilled. If the CAD model includes these features, most CAM systems will attempt to machine them. Typically the result is unwanted areas of toolpath where the tool dives into holes or runs into sharp corners. CAM operators can waste a significant amount of time avoiding and correcting these effects.

Figure 4 - Unmachinable Features

If possible, features that are not to be milled should be excluded from the CAD model used for generating toolpaths. Depending on the type of CAD system being used, this may be done my suppressing features or by covering them with additional surfaces.


Despite years of research, nobody seems to have come up with a concise, accepted definition of HSM or a simple explanation of how it really works. The basic idea is that by taking light cuts at high speed, material can be removed faster than by taking heavy cuts at lower speed. Lighter cuts mean reduced cutting forces, so distortion and vibration effects are reduced. High cutting speeds enable very hard materials to be cut with suitable tooling. High cutting speeds also result in most of the energy of the process being dissipated as heat in the chips, reducing thermal distortion of the part.

None of these benefits will be seen of the machining strategy is inappropriate. Poor strategies usually cause unacceptably short tool life or catastrophic failure. A critical fact to remember is that HSM does not simply mean running existing toolpaths with increased spindle speed and feed rate.

HSM Toolpaths

A toolpath for High Speed Milling has to satisfy a number of constraints. Most of these are obvious when they are written down.

  1. The tool must not gouge the part
  2. The cutting load must be within the capabilities of the tool
  3. The toolpath should leave cusps no larger than the specified limit
  4. Abrupt changes in the rate of material removal should be avoided
  5. Speeds and accelerations must be within the capabilities of the machine
  6. The cut direction (climb/conventional) should be maintained
  7. Sharp changes of direction should be avoided
  8. Non-cutting moves should be minimised
  9. Toolpath execution time should be minimised

However, given a particular part it is often far from obvious how to generate a toolpath that satisfies them all. In fact, it is usually impossible to meet all of these constraints when finish machining real, complex-shaped parts. In this situation we must do the best we can, but where necessary relax one or more of the constraints. Some are clearly more critical than others, and I’ve listed them above in approximate priority order.

Finish machining poses a particular problem for HSM because the shape of the part is a constraint that cannot be relaxed, and compromises in cutting conditions frequently show up as visible marks on the finished surface. Of course these can be polished out, but that undermines the case for using HSM in the first place. Roughing and semi-finishing can be easier to optimise, because the CAM operator has some choice of the shape of the part after the operation, and any marks will be removed by finishing operations.

Programming Capacity

Good HSM programs execute very quickly on the machine tool, but they can take a lot of time and effort to produce. In industries like mould and die making, where parts are produced in one-off quantities, it is common for machines to be held up waiting for programs. Simply pressurising the CAM operators to produce more quickly often leads to corner cutting, with the result that programs are less efficient. In the end a balance is reached where the CAM operators can keep up with the machines, which are running at reduced speed.

Clearly this is not an ideal strategy. To get the best out of HSM it is essential to provide adequate CAM capacity to keep machines fully loaded with high-quality programs.

Planning the Machining Sequence

For anything but the simplest parts, HSM will involve several machining steps. Choosing the right machining sequence is the most important stage of HSM programming and one where experience is most valuable. A significant number of user problems we see at Delcam are caused by inappropriate use of machining strategies, rather than faults in the strategies themselves. The level of automation is increasing steadily in systems like PowerMILL, but in the end there’s no substitute for a bit of careful thought by the user.

It is impractical to describe process planning in detail here, but I will give a few simple guidelines.


HSM places exacting requirements on all elements of the process. It is essential to use the right physical equipment, and this can be specified quite accurately. It is much harder to specify in concrete terms what is required from the CAD and CAM functions; nevertheless these have a significant influence on the quality and stability of the HSM process.

It is essential that CAD models for HSM be prepared to represent accurately the shape that will be milled. This means both that the accuracy of the model must exceed machining tolerances, and also that features that are not to be milled should be excluded from the model if possible.

The investment in HSM equipment must be supported by sufficient programming capacity in order to keep the machines loaded with high-quality programs. Enabling machinists to do some of the programming on the shop floor may be an effective way to boost programming capacity.

Ensure CAM operators and machinists are properly trained and understand HSM thoroughly.

Careful planning of the machining sequence is critical. Making appropriate use of the strategies provided by the CAM system is the best way to get successful results.