CNC Tips and Techniques. Peter Smid
the computer that receives the data (CNC) must be ready before the computer that sends the data (desktop or laptop). That means a bit of running between the two that can be eliminated.
Program Sections
This topics is a very important consideration. Each tool used in the program is automatically a separate section. However, sections for a single tool, especially a tool that does a lot of work, should be carefully defined as well. One technique that can be used is homing the machine (machine zero return) after each section has been completed, particularly along the Zaxis, then starting at the next section with the same tool. As these extra motions add to the cycle time, they should be preceded with a slash (block skip function). An addition of program stop (M00) or optional program stop (M01) to this method may offer additional benefits.
Program Editor
Use a dedicated CNC editor (designed for CNC files) or a text editor that can highlight individual addresses in the program — for example, all Z-axis motions in red. Colors help to identify individual sections, and the editor can also be used to create a temporary copy of a shortened program.
Block or Sequence Numbers
They do help a lot. Although blocks or sequence numbers add to the overall length of the program, this length is irrelevant in DNC operations. If a tool breaks, the sequence number at the time of interruption offers some information that can be used for restart. Instead of using block numbers for each block, consider using only a few block numbers in strategic places within the program. A good place for selective block numbers is at the beginning of every new section that uses the same tool, or at home position.
Descriptive Comments
Identify individual operations or sections of the program. For example, if the same tool is used for roughing five pockets, place a comment at the beginning of each pocket tool path with a unique description.
Feed and Retract Planes
Be consistent in selecting the Z-axis positions for the start of cut and retract when the cut is completed. Text editors can be used to search and/or replace common data.
Cutting Feedrates
If you make the plunging feedrate different from the cutting federate, you will more easily find the beginning of a section from which the change can be done, just by searching for the feedrate. Also, you will not accidentally forget a feedrate or use the wrong one.
What else is there to watch for? The above suggestions can be applied individually, or combined. The most important is to make sure that any change implemented is a safe change. Watch for XY tool locations, missing spindle speeds and feedrates, the status of switches on the control panel, offset settings, and other related subjects.
Running a long program from an external computer in DNC mode can be very simple and uneventful. On the other hand, if problems do arise, be prepared to deal with them via good planning in order to minimize the undesired downtime.
 | Keep Records — Document Your Programs September 2004, updated February 2013 |
There are many reasons to keep track of work done during both common and not-very-common manufacturing processes and activities. The most important reason to keep track of the multitude of activities is to create some reasonable documentation for the work in progress. The method and its purpose are quite basic — to be able to register and retrace or retrieve individual development steps or stages in case of future need. Whether used for emergency purposes or general reference, good documentation is imperative for any serious work in a machine shop environment. At the corporate level, documentation is often developed for internal purposes only. Documentation can also become a major part of the ISO 9000+ certification process, in which case it takes its own form. At the level of CNC or CAD/CAM part programming, the needs in this field are much more relaxed and flexible, but equally important. This essay looks at program documentation relating to CNC programming, regardless of its method of development. Good documentation is as important for manual programming as it is for CAD/CAM tool path development.
Most part programs reach the CNC operator in one of two forms, as a printed hardcopy or as a disc file. In both cases, the program format is the same, only the method of distribution varies. All CNC systems offer a method of inserting comments and messages into the body of the part program. If used properly, these comments and messages are located at strategic locations within the program, as comments intended for the CNC operator. The most common way to include comments and messages in a CNC program is the use of matched parentheses (). This (COMMENT) method is typical for Fanuc and related controls. For example, the following message instructs the CNC operator to check the width of the part:
(WIDTH MUST BE BETWEEN 26.7 AND 27 MM)
Other methods use the dollar sign ($) or the semicolon (;) and similar methods with the same purpose. In all cases, the control system is designed to ignore the message, or comment, during program execution.
Having too many or too few comments in the part program can be counterproductive. Having no comments at all in the program can potentially lead to wrong assumptions, unless some other way of information is provided. The main goal of CNC program comments and messages is to provide an information link between the CNC programmer and the CNC operator. Thorough and informative program documentation is so important that every shop owner or manager should insist upon it and every programmer should provide it as a standard program feature.
Good Program Documentation
What are the main characteristics of good program documentation? The first rule is to make any comment in the program short and to the point. The second rule is to include only those comments that are relevant to the project on hand. In terms of contents or subject matter, here are some suggestions that many CNC programmers have used successfully in various program comments:
Date and Time
The current program version is critical; it must match the part drawing. The latest date and time are assumed to be the latest version.
Programmer’ Name
The programmer’s name is important to the CNC operator in case questions or clarifications are necessary.
Drawing Number and/or Revision
Include the latest drawing version used during the programming process.
Machine Type
A well-developed part program can be used on CNC machines that are similar. A program comment should list which machine/control combinations will accept the given program.
Setup Data
Specify the part zero in all axes. Include the setup method and all related information, such as part orientation, depths, and clearances.
Tooling Data
List all tools at the program beginning and repeat the tool description for each tool in the program.
Special Instructions
If the program contains M00 (program stop), describe the reason for its existence. For example, instruct the CNC operator that the part is to be reversed, or special lubrication has to be applied for tapping, or that the tool has to be checked. Many similar examples fall into this category.
There are many different applications that benefit from comments and messages inserted in the part program. Depending on the control system, the comments may not load into the control memory, but they can always be available in printed form or in the program file. CNC programs developed by CAD/CAM software should include the same comments and messages as programs developed manually. All high level CAD/CAM software offers the insertion of comments into the program.
A well-documented program is easier to interpret by the CNC operator and even by its own author (the programmer). Documentation should be provided as a standard feature of each program.