Conflicting CNC Applications
Almost every critical feature can be used in multiple ways. Be aware of the options, and choose those that are most appropriate for your specific applications.
As CNC application has evolved over the years, CNC providers have developed a variety of ways that certain CNC features can be utilized. Indeed, almost every critical CNC feature can be put to use in multiple ways, and misapplications can lead to under-utilization of CNC machine tools. In some cases, usage methods even conflict with one another, meaning a usage method that works nicely for one company will not be appropriate for another. In order to make the best use of your specific CNCs, you must know your options. Then, you must choose the usage options that are appropriate to your particular company. Here are some common examples of such CNC options, along with a few suggestions for use.
Conventional (offline-programmed) vs. conversational (shop-floor-programmed). This programming decision should be based on three factors: lot size, repeat business and program cycle time. For shops that handle many repeated jobs, large lots and lengthy cycle times, conventional CNCs are the better choice, as there is ample time to prepare programs before they are needed on a machine. When it comes time to run (or rerun) a job, the required program will be ready, and some form of distributive numerical control (DNC) system can be used to quickly transfer it to the CNC.
Conversely, shops that consistently run small lots of new jobs with short cycle times often find it impossible to keep up with the number of required programs. Programs are almost always created while the machine is down between jobs. In these situations, conversational CNCs programmed on the shop floor often shorten programming time and eliminate the need to transfer programs.
Cutter compensation offset specification (cutter diameter vs. cutter radius). With newer CNCs, this selection is a parameter setting. Older CNCs offer no choice, so you will be stuck with the method provided by the CNC manufacturer. If you have both older and newer machines, it may be better to maintain consistency and select the method used by the older machines for the newer ones. Otherwise, this decision should be based on how much sizing your setup people and operators perform with cutter compensation.
For the initial entry, and if the work surface path is programmed, specifying the cutter diameter is much easier than specifying the radius. If a cutter is 1 inch in diameter, the initial offset entry will be 1.0 (using the imperial measurement system). With radius measurement, the initial entry will be half the cutter diameter. If the initial setting is the only consideration, choose diameter entry. However, sizing adjustments are more difficult with diameter entry, since the adjustment amount must be doubled each time. If 0.001 inch more material must be removed from a workpiece surface, for instance, the adjustment amount will be -0.002 inch. With radius entry, the adjustment amount will match the amount of material that must be removed from the workpiece surface (-0.001 inch for this example).
Cutter compensation offset specification (cutter size vs. deviation from planned size). This decision is based on whether a CAM system is used to create programs, as well as whether the “planned” cutter size is used. If the programmer specifies the work surface path, the initial offset setting will be the cutter size (radius or diameter). If the programmer specifies the cutter’s center line path, and if the planned cutter size is used, the initial offset setting will be zero. CAM systems can generate either cutter center line path or work surface path; it is simply the programmer’s choice.
On the other hand, manual programmers writing with G code usually find it more difficult to program the cutter’s center line path and tend to program work surface path instead. Since the initial adjustment is easier when programming the center line path (zero, if the planned cutter size is used), this is our recommended method if a CAM system is used to create the CNC program. Sizing adjustments are done in the same manner regardless of which programming method is chosen.
Tool-length compensation offset specification (cutting tool length vs. distance from tooltip to Z-axis program zero surface). This decision is based on lot sizes, cycle times, how often the same cutting tools are used from job to job and the availability of support personnel. The more time there is during one job to get ready for the next job, the more important it is to use the cutting tool’s length as the offset value.
The tool length is the distance from the tooltip to the spindle nose, a positive value. This length can be measured either on the machine or offline, it will remain consistent from one job to the next, and it will even remain consistent among multiple machines. For these reasons, we recommend using the cutting tool’s length as the tool-length compensation offset value. With this method, the Z-axis program zero assignment value, the work coordinate system offset Z register value, will be the distance from the spindle nose to the Z-axis program zero surface (a large, negative value).
Even if there is limited preparation time and cutting tool lengths must be measured during setup, it is just as easy to measure a cutting tool’s length on the machine as it is to measure the distance from the tooltip to the Z-axis program zero surface. If cutting tools are often used from job to job, using the cutting tool length as the tool-length compensation offset value will save the duplicated effort required for measuring.
They offer benefits that many CNC users overlook.
The relationship between these two basic departments is critical to the success of any manufacturing company.
Which command is better to get your machine axes to the reference position?