the CAD/CAM system is another equally important component. Today’s CAD/CAM systems have greatly advanced over the years,

providing a wide variety of system tools and capabilities. Furthermore, development continues to grow at an outstanding pace. However, not all of today’s systems are created equal and it is important to realize that there are still many systems that do not have the built-in tools or strategies to create toolpaths for hard milling or HSM.

Although no system is devoted entirely to hard milling, many that offer HSM capabilities will have the same strategies for hard milling since there is a common relationship between the two technologies. When considering hard milling, strategies that keep the tool in motion should be used for hard milling.

This will ensure that the tool is continuously cutting with a constant chip load. This is one of the more desirable conditions to maintain for hard milling. Before further discussion on machining strategies can begin, a careful review of the CAD model is important.

One of the common problems associated with CAD/CAM programming is the model. Many companies import data from other systems using a variety of importing tools. In particular, job shops may deal with various clients, who are using a variety of different CAD systems. In this case, a file transfer format needs to be defined to transfer geometry data from the client CAD system to the CAM system. In order to avoid time-consuming repairs of the model, it is very important to select the proper file format for a data transfer.

Some CAM systems offer special interface options to directly read in file formats from other CAM systems. When data is imported, problems can pop up. These problems range from missing trimmed surfaces to bad solid models causing numerous headaches for creating efficient toolpaths. These problems need to be fixed before developing toolpaths.

Poorly developed models also are a common problem. Typically, how a model is created is going to dictate what machining techniques are used. If machining strategies are not considered during the development of the model, then the programmer may not be able to use certain toolpath strategies. Without these considerations, hard milling a cavity or core may not always be suitable without modifying the model. .

Before toolpaths can be applied, there must be a complete analysis of the part. Not all parts are suitable for hard milling. The specific areas to be machined should be clearly identified, determining the smallest internal radius and largest working depth. A 4:1 ratio of length to tool diameter commonly does not pose any problems.

Problems arise when the ratio grows, and careful consideration should be made towards the feasibility of success. When ratios are excessive, experience at hard milling will have an important role in determining how successful one will be.

Hard milling with tool diameters as small as 0.005″ can be accomplished as long as care is taken to maintain a constant chip load and machining at minimal cutting depths. These depths can commonly range from 0.0002″ to 0.0005″ on such small tools. Toolpath strategies can now be determined.

As mentioned earlier, in hard milling it is important to keep the tool in motion avoiding dramatic changes in direction. Therefore, depending on the complexity of the part, multiple toolpath strategies may be required to complete the part.

The process of recognizing and separating key areas of the part and applying different toolpath strategies is commonly called modular toolpath programming (MTP). This method of programming is generally used in HSM to maintain high cutting speeds. Similarly, MTP can be used to help keep the tool in motion while avoiding dramatic changes in direction. Although simple, this is not the ideal method for machining this part in its hardened state.

If individual part features are recognized and separated, two different strategies can be applied to this part . In this simple example, a spiral morph toolpath on the green surface, combined with a true spiral from top to bottom on the red surface, provides a suitable method for machining this part. Toolpath quality is commonly overlooked in a CAM system. but upon further evaluation, it is revealed that there are many unnecessary changes in the toolpath direction .

Stepping back to our machine tool, builders have incorporated elaborate acceleration and deceleration servo tuning algorithms as well as complex servo lag algorithms (look ahead features) into their controls to enhance motion control. These look ahead or control feedrates by analyzing directional changes within the NC code.

The greater the directional change (for example, zero to ninety degrees) the more the control has to slow down to maintain the programmed path. In hard milling, these abrupt changes in toolpath direction create dwells and slow downs, which can have an effect on tool life and surface finish. Therefore, toolpath quality should be an important feature of your CAM system.

Programming errors have a tendency to be less forgiving when conventional machining techniques and softer materials are used. With hard milling and HSM, programming error will no doubt have severe consequences if not caught in time.

Cutting tools can easily be broken; tool holders, fixtures and even the machine can be damaged costing hundreds to thousands of dollars. Personal safety also can be at risk. To ensure programming errors are caught before they happen, the CNC code should be thoroughly reviewed for errors. Most CAD/CAM systems incorporate some type of toolpath verification or toolpath simulation within their software. Unfortunately, many of them only view the intermediate file rather than the posted NC code or the C/L toolpath file where errors can occur.

Therefore, care should be taken to ensure that the posted NC code is reviewed for errors. If your CAD/CAM system does not have the tools to view or simulate the NC code directly, there are numerous software packages on the market that will. These products can range from a few hundreds dollars to several thousands of dollars but they will save you many major problems by eliminating potential crashes and safety issues at the machine.

Know-how
Finally, proper know-how and training are vital keys to being successful at hard milling. You can have all of the above elements but they are no good to you without a clear understanding of principle processing procedures. Often, an entirely new approach is required to gain the profitable advantages of the hard milling process over conventional milling.

The successful employment of the hard milling process is based on specific know-how, advanced knowledge of the basics of the HSM process, choice of appropriate cutting tools, choice of appropriate clamping systems for cutting tools (and parts) and professionalism, using an HSM capable CAD/CAM system.

There are many resources for hard milling. The supplier or OEM should be your first choice. For example, a cutting tool representative will be able to assist in selecting the correct feeds and speeds for a particular cutting material. Many work directly with machine tool builders for adequate testing of their tools.

Manufacturers of tool holders commonly work with builders to share and gather information regarding equipment performance. This also holds true for CAD/CAM developers who commonly work closely with machine tool builders testing new machining strategies and sharing ideas on new and improve machining methods. Training must be on a continuous basis.