a lot simpler and less tedious; having support for them in the CAM software makes it easier at the machine to make small machining changes. Some CAM software offers an open architecture model. In plain words, it means that anybody with the required skills can write special utilities that can be accessed by the CAM software. The ability to add external features greatly adds to the power of the CAM software.
Multi-Machine Support
Some machine tool manufacturers provide their own CAM software dedicated only to the CNC machines they make. Typical examples in this area are fabricating machines and some EDM machines. The software usually performs very well for the machine type supported, but it lacks flexibility to support other machines. It is quite suitable for a specialized shop, but not very practical for a shop that needs programming flexibility.
Most CAM software is integrated software, which allows the part programmer to use it for several types of machine tools, typically mills, machining centers, and lathes. The major advantage of integrated CAM software is its flexibility. Additional benefits may be more practical, but also important, for example, a similar interface for milling and turning shortens the programming time.
Text Editor
In many respects (and professional opinions), the text editor that is supplied with most CAM software should be only a viewer — it should not be able to make changes to the program. Of course, such changes are made every day because it is an expedient way to fix a problem, usually a minor one. The program generated by CAM software should not need editing; that is the whole purpose of purchasing it in the first place. Yet, many part programmers choose to make small changes manually. In principle, it is a wrong approach. The problem may have been fixed, but the program database, the part model, has not changed at all. It still contains the error. In an environment when several users work with the program, this approach can cause major difficulties.
At the same time, a text editor does have its own legitimate uses. For example, the editor can create and edit setup and tooling sheets, post processor templates, even configuration files. None of these applications will cause damage to the toolpath database. A text editor can also be used to print the program if hard copy is required.
CAD Connnection
A stand-alone CAM programming system does not require separate CAD software to define toolpath geometry. If a part drawing already exists (for example, if the customer delivers an Autocad drawing as a file), it is counterproductive to redraw the geometry. The CAM software should contain several built-in CAD conversion features. Autocad is still the leader in 2D drafting, and opens DWG drawings directly. DXF format is also available, but only suitable to translate basic entities. For 3D design, quality CAM software should convert the most popular CAD systems, such as Solidworks, Inventor, Catia, and SolidEdge. Others are added frequently.
Managing a CAM System
CAM software requires a certain organization to support it; it needs planned strategies and focus. CAM system management establishes standards and procedures for all users, be it at the simple level of naming files to developing tool and material libraries, backup methods, and data security.
Training and Technical Support
Unfortunately, training is often neglected, even ignored. Professionally conducted training sessions will produce measurable positive results in a relatively short time. Most CAM vendors provide basic level training; some offer more specialized training. Initial training is usually general in nature, and should be provided to the person who has previously programmed manually. Any training should be practical in its orientation, preferably the usage of actual parts. A quality training program should also include short follow-up sessions that address problems encountered and answer many questions.
Technical support for CAM software is as important as for any CNC machine or control in the shop. A service or software maintenance contract is offered by many vendors, assuring of the latest updates and improvements, at a reasonable cost.
 | Minimizing Program Length May 2005, updated February 2013 |
In the past, the topic of handling long programs has focused on running such programs efficiently at the machine, during the actual part production with DNC support. Long programs are often the result of a CAM output, but they are also developed manually in many cases. Keep in mind that the word long is quite often relative to the amount of work involved and the available control memory capacity. CNC lathes, for example, have much smaller memory capacity than CNC machining centers. In either case, CNC programmers have several methods at their disposal that will make long programs shorter. Using the methods suggested in this column, it may often be possible to fit a long program into the control memory, without using the DNC method. Various methods are available to reach this goal and they can be adopted before the program is developed or after the program has been developed.
In CAM programming, the main key to quality program output is a quality post processor. The purpose of a post processor in CAM software is to provide a customizable platform for the desired program output. The same thoughts and efforts that go into post processor customization will also be considered in manual programming. There is no magic here — if you want to shorten the program, you must do it without losing its integrity and purpose. Removing an operation from a program will certainly make the program shorter, but the price may be too high to pay. When developing the CNC program, look at various features that offer shorter output right from the box, so to speak. They include various fixed cycles, multiple repetitive cycles, subprograms, macros, counters, and automatic corners. Starting with a program that is already as short as possible, it makes any subsequent effort that much more effective. Let’s look at some options available.
Eliminating Characters
Once all possible methods have been used to make the program shorter from the beginning, there is only one more method left — to eliminate all unnecessary characters from the program. Yes, eliminating one character at a time will often work miracles on the final program length. You will need a good text editor, preferably one designed for editing of CNC files. Text editors offer feature called mass substitution (commonly known as the find and replace feature). Always work on a copy of the program, in case something goes wrong. Also, never make changes to the program that would negatively affect machining safety. Initial planning is important and the knowledge of program formatting is imperative. Here are the main areas that should be considered as methods suitable for the reaching the goal of a shorter program:
• Elimination or optimization of block numbers (sequence numbers)
• Removing program comments
• Removing unnecessary zeros
• Joining single-axis motions into multi-axis motions (if safety allows)
Block Numbers
Block numbers are almost always used for convenience, except in some special applications, such as multiple repetitive cycles or macro statements. Eliminating block numbers will make the most significant reduction in any program size. If you don’t feel comfortable about eliminating all block numbers, use only one block number per tool, perhaps for the purpose of searching. Using block numbers in increments of one is more economical that common increments of five or ten, as fewer characters are stored.
Comments
If the control system accepts comments and messages within the program (those enclosed in parentheses), a great amount of available memory is used by them. Eliminating — or at least minimizing — the use of comments in a program will also go a long way to a shorter program.
Unnecessary Zeroes
Removing unnecessary zeros from the program may take a little