4 Commonly Misapplied CNC Features

CNC machining centers and turning centers are used for countless applications, which is why almost every manufacturer has these machines in their shops. Paralleling company diversity is the wide spectrum within each utilization factor:

• Lot size – At one end of the spectrum are companies that regularly run under 10 workpieces per lot. At the other end are companies that dedicate CNC machines to running one part, day in and day out.
• Repeat business – Some companies repeatedly run a finite number of different workpieces, while others never see the same job twice.
• Lead times – Some companies have days, weeks or even months to get ready to run jobs, while others must provide same-day services.

I consider these among the most important utilization factors. Others that vary among CNC users include profitability, tolerances held, materials machined, available personnel/skill levels, average setup time, average program execution time and complexity of work. With a little thought, you can probably come up with several more.

Knowing these diversities exist, CNC manufacturers do their best to provide features aimed at satisfying all of their customers. Indeed, some features are important to and appreciated by everyone. Features like decimal point programming, radius designation for circular motion and hole-machining canned cycles can be regularly applied without negative side effects.

Other CNC features are not so benign. The CNC manufacturer may be targeting a niche application, like small lots or often repeated jobs, or helping with unique setup-related issues. Misapplication of these features will result in wasted time, wasted or duplicated effort and/or wasted material (scrap). Here, I expose four such CNC features as well as how and when they could be misapplied. More importantly, I ask you to consider other misapplications that may exist in your own shop.

Conversational controls

These controls enable shopfloor programming. They are best applied when the machine commonly runs small lots of seldom repeated jobs; relatively simple workpieces with short to medium program execution times; and especially when one person is responsible for everything related to the job, including programming. Many contract shops have machines matching these criteria.

As lot sizes grow and jobs are repeated — with more complex workpieces requiring longer run times and/or when more people are available to help with the CNC process — the benefit of shopfloor programming fades. Companies with this scenario, like many product producing companies, tend to have workers specialize in the tasks they perform. Many tasks are performed in preparation for upcoming jobs while the machine is running the current job. This includes the task of programming. For them, using a conversational control wastes precious machine time.

Tool length compensation

There are two ways to use machining center tool length compensation. While programming remains the same for each, operation techniques are dramatically different. The best method for your shop is largely determined by how CNC people are utilized.

With one method, the tool length compensation value is the distance in the Z-axis from the tool tip to the Z-axis program zero surface. It is measured during the setup, meaning the machine must be used as a kind of (very expensive) height gauge. This is only appropriate if tool length compensation values must be measured by the operator while the machine is down between production runs, which is often the case in contract shops.

With the other method, the tool length compensation value is the tool’s length. Assuming the company has the resources (personnel and tooling components), cutting tools can be assembled and measured, possibly in the tool crib, while the machine is in production. Tool length compensation values entry can even be programmed, commonly by the tool length measuring device. Related setup time is reduced to the time it takes to load the program and execute it once.

Fixture offsets

There are two ways to use fixture offsets based on whether setups are qualified (aligned with the machine table in such a way that the workholding device can be precisely placed and replaced). If there is very little repeat business for a machine, it can be difficult to justify the extra cost related to qualifying a workholding setup.

With one method, used with workholding setups are not qualified, the setup person must measure the distance in each axis from the machine’s reference position to the program zero surface for the axis. These values are manually entered into the related fixture offset registers. They must be remeasured every time the setup is made.

With the other method, which should be used when setups are qualified, the program zero assignment values will remain the same from one time the setup is made to the next. A programmed command can be used to enter these values into the fixture offset. With FANUC CNCs, it is even possible to shift the point of reference for fixture offset entries from the machine’s reference position to a more logical location, which is especially helpful when using subplates and component tooling. Either way, this second method eliminates the entire task of program zero assignment.

Tool nose radius compensation

With FANUC turning center CNC-based tool nose radius compensation, the CNC programmer uses G41 or G42 to specify the relationship between the cutting tool and the workpiece. The setup person must specify, with offset settings, the type of tool (turning tool, boring bar and so on) and its nose radius.

This feature and its method of use work well when CNC programs must be manually written at G-code level. But when a CAM system is used to prepare programs, the programmer can specify the cutting tool’s nose radius and the CAM system will generate a compensated tool path. This eliminates the need for the operator to make the offset entries previously mentioned, which in turn, reduces setup time and the potential for entry mistakes.

To summarize, serious waste will occur when:

• A company that has lots of repeat business, predictable lead times, lengthy program execution times and complex work uses conversational controls for programming.
• A company that has adequate resources requires their setup people to measure cutting tool lengths on the machine during setup.
• A company that consistently makes qualified setups requires setup people to measure program zero assignment values every time a job is run.
• A company that uses a CAM system to prepare programs uses CNC-based tool nose radius compensation, requiring setup people to enter related values into offsets.

I urge you to relate these considerations to other CNC features you are using. Make sure that you are applying them appropriately to your company’s needs.