CNC tezgahlarda parametrik programlama

Abstract

Dünyada, bilgisayar alanındaki hızlı gelişmeler, Takım Tezgahlarında da bilgisayarın kullanım alanının artmasına sebep olmuştur. Ülkemizde de yaygın olarak kullanılmaya başlanan CNC tezgahlarda, her makinayı kontrol eden bir operatör bulunmaktadır. însan faktörünün en aza indirgendiği ve tam otomasyonun gerçekleştirilebildiği sistemlerde, CNC tezgahlar, insan müdahalesinin az olabileceği şekilde programlanmalıdır. Buda "CUSTOM MACRO" olarak bilinen parametrik programlama ile yapılabilir. CNC Tezgahlarda programlama için, her bir fonksiyonu ifade eden çeşitli komutlar kullanılır. Bu komutlar adres olarak tanımlanan bir harf ve onu ta kip eden rakamlardan oluşur. Bu komutlar parça resmi ve kullanılacak kesici takımlara göre belirli bir sırada düzenlenerek parça programı oluşturulur. Custom Macro programlamada, bilgiler gurubunu içeren bir fonksiyon, alt program şeklinde hafızada saklanır. Custom Macro yapısını oluşturan bu bilgiler gurubunda, değişkenler, değişkenler üzerinde ger çekleştirilebilen işlemler ve Custom Macro bilgileri içindeki değişkenlere atanabilen gerçek deçerler mevcuttur. Custom Macro programlama ile karışık şekle sahip parça programları daha kolay yazılabildiği gibi, robot mekanizması ile çalışan tezgahlarda, takım aşınması sonucu oluşabilecek kazalara sebebiyet vermemek için takımların belirli periodlarla ölçülmesi, belirli parça sayısından sonra makinanın durması gibi fonksiyonları gerçekleştirmek mümkün olmaktadır. işlem merkezlerinde takım değiştirme, takım boyu ölçme gibi işlemler, Custom Macro yapısında oluşturulmuş alt- programlar şeklinde hafızada bulundurulup, tek bir program komutu ile çağırılarak fonksiyon gerçekleştirilebilir.

The Outline Of The Programming : Before making correct programming for varius types of jobs, some procedure has to be considered. From the origi nal drawing of workpiece, style of part dimensioning is changed for easier programming. Cutting sequence, cutting direction and chucking location are planned. In respect of cutting speed, depth of cut and feedrate, cutting condition are determined and cutting tools are selected. According to cutting area for each cutting tools, the program is writen by using standart programming commands. For program configuration, a group of commands given to the NC for operating the machine is called the program by specifying the commands, the tool is moved along a straight line or an arc, or the spindle motor is turned on and off. A group of commands at each step of the sequence is called the block. The program consists of a group of block for a series of machining. The number for discriminating each block is called the sequence number and the number for discriminating each program is called the program number. Each block consists of a sequence number for indicating the NC operation sequence at the beginning of the block, prog ram command including an adress and the number specifies a function and a CR code for indicating the end of the block. v The Program Format : Following explanation are for the addresses and the instructions for program format use. Address Function The Instruction for their use Program Number Designated by 4-digits number following the address O N Block Number Designated by a maximum 4 -digit (Sequence Number) number (usually 3-digits no.) following the address N Preparatory Function Designated by a 2-digits number following the address G. The motion of the slides can be programmed by using the G codes Feed Function The feed function directly designates the amount of feed per revolutions of the spindle. Spindle-Speed Function Specifies the amount of spindle speed in r.p.m. surface speed in meter per a minute. T Tool Function T specifies the selection of the turret station and the tool offset number. M Miscellaneous Function Designated by a 3-digits number following the address M for specifying auxilary function, such as spindle start and spindle stop. VI p u X Dwell Specify the number of dwell time by using 8-digits number following the address P, used with code GO 4. Radius of arc Specify the value of the radius when using G01, G02 or G03. The points of movement in the X-axis Specify the absolute coordinate point in the X-axis. u The points of Specify the relative coordinate movement in the point in the X-axis. X-axis The points of Specify the absolute coordinate movement in the point in the Z-axis Z-axis W The points of Specify the relative coordinate movement in the point in the Z-axis Z-axis / Block Skip When the "Block delete" switch is set to ON position, the commands of a block containing "/" will not be executed. (CR) End of Block Designates the end of a block. The coordinate zero point (work coordinate zero point) is determined to be any place such as the face of chuck, the face of the part etc. However the face of the work- piece on chucking work and cut-off face on bar work are convenient. vxi 6 - Function ( Preparatory Function ) : The G code indicates a 2 digit number following the address G for specifying the motion of the slides such as linear or circular. Standart G codes used for the program ming of CNC lathes are as follows. 6 00 : Positioning ? This command is used for the positioning of tool by moving at a rapid traverse rate for each slide direction. 6 01 : Linear Interpolation ; A tool is moved on a straight line at a feedrate specified by the F code. 6 02, 6 03 : Circular Interpolation ; When G 02 or G 03 is commanded, a tool is moved along an arc at a feed- rate specified by F code. Arc radius is given by R command. Rotation direction of G 02 is clockwise and G 03 is counter clockwise. 6 04 : Dwell ; The feed can be stopped for a designa ted period of time by programming this command. 6 10 : Changing of tool offset amount ; This command is used to input offset values by a program. 6 20, 6 21 : Inch / Metric Input ; Either inch or metric input can be selected by these codes respectively. 6 28 : Automatic return to reference point ; The tur ret slide is moved at a rapid traverse rate for each direc tion simultaneously to the reference point. G 32 : Thread cutting ; Straight, taper and face thread cutting are effected by using this command. 6 50 : Spindle Speed and Coordinate Setting ; This command is used for setting of maximum spindle speed and coordinate system setting. 6 96 : Constant Cutting Speed Control ; When S code is commanded in G 96 mode, the number following the addres S specifies the cutting speed as being meter per minute. 6 97 : Constant Cutting Speed Control Cancel ; In this mode S command specifies the spindle speed in RPM. 6 98 : Feed rate per minute G 99 : Feed rate per revolution vm H - Function ( Miscellaneous Function ) : The M Function is designated by using 2 digits number following the address M for specifying an auxilary function M 00 : Program Stop ; When M 00 is commanded in auto matic operation mode, the automatic operation will stop af ter completion of the commands in the block containing M 00 M 01 : Optional Stop ; This is usually used to stop the machine and check workpieces at the end of each tool operations. M 02 : End of Program ; This code is used in the last block of program to end the program. M 03 : Spindle Forward ; Specifies to start the main spindle rotation in counter-clockwise direction. M 04 : Spindle Reverse ; Specifies to start the main spindle rotation in clockwise direction M 05 : Spindle Stop ; Specifies to stop the main spindle rotation. M 08 : Coolant ON ; Specifies to start the coolant M 09 : Coolant OFF ; Specifies to stop the coolant M 30 : Program Stop ; Specifies at the last block of the program. M 98 : Subprogram Call ; This code is used to enter a subprogram. M 99 : End of Subprogram ; This code shows the end of program. Custom Macro Programming : In custom macro programming, a function covering a group of instructions is stored in memory as a subprogram. The stored function is represented by one instruction, so that only the representative instruction need be specified to execute the function. This group of registered instruc tions is called a "custom macro body" and the representa tive instruction is called a "custom macro instruction". IX The custom macro body may simply be called Macro. And the custom macro instruction may be called a macro call command. The three most significant points on custom macros are that variables can be used in the custom macro body, opera tions can be performed on variables and actual values can be assigned to the variables in custom macro instructions. In order to call custom macro body, custom macro com mand is used. It is possible to call the subprogram by using M or T code by setting related parameters. Usually M 98 code is used to call custom macro. In the custom macro body, the CNC command which uses ordinary CNC command variables, calculation and branch command can be used. The custom macro body starts from the program No. which immediately follows 0 and ends at M99. Instead of directly providing a numeral to an address in the custom macro, a variable can be specified to make the macro flexible and versatile by applying the calculated variable when calling the macro. Variables are sorted into common variables and system variables according to variable numbers. Common variables are used to change or calculate the exact program command. System variables are used for input and output signals, tool offset amount, clock confirmation, number of necessary parts and machined parts, modal information and position information.