Quality Control Check Sheet
This planning document is used for the final inspection stage of the machining process. Once the part is completed, it is necessary to check all of the dimensions listed from the engineering drawing or blueprint to verify they are within the specified tolerance. The Quality Control Check Sheet is an excellent method to document the results of this inspection and a valuable tracking tool.
Reference information is similar to the other planning documents. Included are:
• The date the document is prepared or revised
• The name of the person checking the part
• The part name and part number (from the engineering drawing or blueprint).
On the check sheet, 100% of the engineering drawing or blueprint dimensions and their tolerances are written down in list form. Using this method, sequentially go through each of the dimensions and log the results. This assures that the machined part meets the specifications given on the engineering drawing or blueprint. As the part is checked and verified, some dimensions may not meet specifications. It is important to identify these incorrect values, emphasizing them for correction whether with red ink or a highlighter pen (or by changing font color or highlight if in electronic form). You could also include details in the comments section of the QC Check Sheet (Chart 1-3). If dimensions are found that do not meet specifications, corrective action must be taken.
Chart 1-3Process Planning Quality Control Check Sheet
| Date | Checked By | ||
| Part Name | Part Number | ||
| Sheet ___of ___ | |||
| Blueprint Dimension | Tolerance | Actual Dimension | Comments |
TYPES OF NUMERICALLY CONTROLLED MACHINES
There are two basic groups of numerically controlled machines: Numerical Control (NC) and Computer Numerical Control (CNC).
In an NC system, the program is run from a punched tape where it is impossible to store such a program in memory. For a punched tape to be used again to machine another part, it must be rewound and read from the beginning. This routine is repeated every time the program is executed. If there are errors in the program and changes are necessary, the tape will need to be discarded and a new one punched. The process is costly and error prone; although this type is still in use, it is becoming obsolete.
Machines with a CNC system are equipped with a computer, consisting of one or more microprocessors and memory storage facilities. Some CNC machines have hard drives and are network configurable. Program data is entered through Manual Data Input (MDI) at the control panel keyboard, via an RS232 communications interface port or via Ethernet from a remote source like a personal computer (PC) network or from a USB drive. The control panel enables the operator to make corrections (edits) to the program stored in memory, thereby eliminating the need for new punched tape.
Types of CNC machines have expanded vastly over the last decade. Turning and machining centers are the focus of this book, but there are many other types of machines using Computerized Numerical Control. For example, there are: multi-task mill turn centers, electrical discharge machines (EDM), grinders, lasers, turret punches, and many more. Also, there are many different designs of machining and turning centers. Some of the machining centers have rotary axes and some turning centers have live tooling and secondary spindles. For this text, the focus will be limited to vertical machining centers with three axes and turning centers with two axes. These types of machines are considered the foundation of all CNC learning. All operations on these machines can be carried out automatically. Human involvement is limited to setting up, loading and unloading the workpiece, and entering the amounts of dimensional offsets into registers on the control.
CNC programming is a method of defining machine tool movements through the application of numbers and corresponding coded letter symbols. As shown in the list below, all phases of production are considered in programming, beginning with the engineering drawing or blueprint and ending with the final product:
• Engineering drawing or blueprint
• Work holding considerations
• Tool selection
• Preparation of the part program
• Part program tool path Verification
• Measuring of tool and work offsets
• Program test by dry run
• Automatic operation or CNC machining
Begin all programming by closely evaluating the engineering drawing or blueprint; emphasizing assigned tolerances for particular operations, tool selection, and the choice of a machine. Next, select the machining process. The machining process refers to the selection of fixtures and determination of the operation sequence. Following that, select the appropriate tools and determine the sequence for their application. Before writing a program, calculate the spindle speeds and feed rates.
When program writing begins, give special attention to the specific tool movements necessary to complete the finished part geometry, including non-cutting movements. Identify individual tools and note them in the program manuscript. Also note miscellaneous functions for each tool such as: flood coolant, spindle direction, r/min and feedrates (these items will be covered in greater detail in the following chapters). Then, once the program is written, transfer it to the machine through an input medium like one of the following: punched tape, floppy disk, USB, RS-232 interface, or Ethernet.
Initiate the machining by preparing the machine for use, commonly called setup. For example, measure and input workpiece zero and tool length offsets into CNC memory registers. Many modern controllers have a function for graphical simulation of the programmed tool path on the cathode ray tube (CRT). This enables the machinist or set-up person to verify that the program has no errors, and to visually inspect the tool path movements. If all looks well, machine the first part with increased confidence. After completion, a thorough dimensional inspection will compare dimensions