螺旋插补教程

螺旋插补例程在Turbo PMAC控制器中，螺旋插补仅仅是标准圆弧插补的扩展，不执行圆弧插补的轴将自动执行线性插补运动。

在螺旋插补中，一般使用X,Y作为圆弧插补轴，Z轴为直线轴垂直于XY平面，如果添加一个与圆弧平面垂直的旋转轴C，使刀具与运动路径成一个固定的夹角，可以保证刀具始终垂直于切割面。

例如，完成一个XY平面的起点为（X=10,Y=0）的完整圆，可以使用下列命令：NORMAL K-1 ；指定XY平面，Z轴为垂直轴CIRCLE2 ；逆时针圆弧插补ABS ；按坐标指定终点（绝对模式）INC(R) ；按圆心指定终点（相对模式）X10 Y0 I-10 ；开始圆弧运动如果没有给出一个轴的明确终点，则认为终点与起点重合，在圆弧插补中，若未定义圆弧终点坐标，默认会执行完整的圆弧，所以执行画圆的指令可以简化为：I-10加入Z轴，使其运动到Z=1，C轴为旋转轴旋转至360°，命令可变为：X10 Y0 I-10 Z1 C360由于是一个完整的圆，指令可简化为：I-10 Z1 C360应用实例有时，内螺纹太大无法进行攻丝，这就需要一个可以三维平动并可自身旋转的单点刀具，以确保紧贴并垂直于内表面进行切削。

这些直角坐标轴执行螺旋插补，旋转轴则以恒定角速度运动。

为确保满足切削深度并保护刀具，程序需要执行一系列“回合”，执行每个“回合”都会增加一定切削深度，一个“回合”是一段螺旋插补，专门完成一段螺纹，在各段之间使用Rapid运动以准备下个段的插补。

每个圆弧运动模式周期都会在XY平面产生一个完整的圆，Z轴会运动一个“螺距”，而C轴也会运动360°。

程序速度是刀具中心在XYZ空间的矢量速度（默认为Frax （X,Y,Z）命令）。

这个速度会在程序中分解到各轴，因为刀具中心的速度要慢于刀尖的速度。

可以在示例中使用刀具半径补偿，补偿方式在程序中隐含。

下图是螺旋插补的正视图和侧视图。

如下设置及程序可实现上图所示运动; Set up coordinate system设置坐标系&1 ；指定坐标系1#1->400X ；X(mm)2.5um分辨率#2->400Y ；Y(mm)2.5um分辨率#3->400Z ；Z(mm)2.5um分辨率#4->100C ；C（角度）0.01°分辨率I428=36000 ；#4（C）整圈3.6万ctsI5113=10 ；坐标系1粗插补10msI5190=60000 ；坐标系1速度6万cts/ms定义#define CenterX Q500 ；孔中心X坐标#define CenterY Q501 ；孔中心Y坐标#define RetractZ Q502 ；起刀位Z坐标#define StartZ Q503 ；切削开始Z坐标#define BottomZ Q504 ；孔底部Z坐标#define Pitch Q505 ；螺距（用户单位）#define ToolCenterRad Q506 ；刀具中心运动半径#define InsideRad Q507 ；未切削孔半径#define DepthIncr Q508 ；每“回合”切削深度#define ToolLength Q509 ；刀具中心距刀尖距离（刀具长度）#define ThreadDepth Q510 ；最终应达到的切削深度#define ThreadNum Q511 ；螺纹切削计数#define NumOfThreads Q512 ；总的螺纹数#define CutSpeed Q513 ；刀尖切削速度；设置系统常量RetractZ=450 ；起刀位距起始位置450mmToolLength=25 ；刀尖距刀具中心25mm；设置切削参数CenterX=-220 ；距起始位置（单位：毫米）CenterY=135 ；距起始位置（单位：毫米）BottomZ=20 ；距起始位置（单位：毫米）Pitch=10 ；螺距（单位：毫米）InsideRad=55 ；距孔圆心距离（单位：毫米）DepthIncr=0.2 ；每回合增加的深度（单位：毫米）ToolLength=25 ；距刀具中心（单位：毫米）ThreadDepth=8.0 ；距未切削表面（单位：毫米）NumOfThreads=10 ；完整圆弧个数（螺纹数）CutSpeed=80 ；切削速度单位：mm/minOPEN PROG 60 CLEARRAPID ；快速模式ABS ；所有轴均为绝对模式X(CenterX) Y(CenterY) Z(RetractZ) C0 ；到达孔入口处StartZ=BottomZ-Pitch/10Z(StartZ) ；Z到达开始切削位置ToolCenterRad=InsideRad+DepthIncr-ToolLengthX(ToolCenterRad) ；刀具中心运动至理想刀具中心运动半径FRAX(X,Y,Z) ；矢量速度中包含的轴；循环中螺纹数加1进入下一部分WHILE (ToolCenterRad+ToolLength<InsideRad+ThreadDepth)ThreadNum=0WHILE (ThreadNum<NumOfThreads+1)CIRCLE2 ；逆时针圆弧模式F(CutSpeed*InsideRad/(InsideRad-ToolLength))INC(Z,C) ；这些轴为增量模式I(-ToolCenterRad) Z(Pitch) C360 ；X,Y运动一个完整圆弧，Z轴运动一个螺距，C轴旋转360°ThreadNum=ThreadNum+1 ；螺纹计数+1ENDWHILERAPID ；快速进入下一段ABS(Z) ；绝对模式X(InsideRad-DepthIncr-ToolLength) ；清除孔内余物Z(StartZ) ；Z轴回归起刀位ToolCenterRad=ToolCenterRad+DepthIncr ；进入下一段X(ToolCenterRad) ；运动到下一个切削深度ENDWHILEX(CenterX) Y(CenterY) Z(RetractZ) ；归原位CLOSE使用G代码执行通常操作类似于螺纹切削会使用子程序，在G代码程序中，这种类型操作被称为“固定循环”由一个含有一系列代码参数的程序调用，在这个例子中，我们可以使用带有8个参数的G78代码调用，在下面给出：G78 X Y Z R P T D IX的值是孔圆心的X坐标Y的值是孔圆心的Y坐标Z的值是孔底部的Z坐标R的值是孔内部半径P的值是螺距T的值是螺纹计数D的值是期望切削深度I的值是每“回合”切削深度在Turbo PMAC中G代码子程序在Prog1000中定义，子程序每行前加入100倍于G 代码数字的标号，例如G78的子程序会调用Prog1000中的标号为N78000的行。

；参数替换及定义#define XArg Q124 ；X值传递变量#define YArg Q125 ；Y值传递变量#define ZArg Q126 ；Z值传递变量#define RArg Q118 ；R值传递变量#define PArg Q116 ；P值传递函数#define TArg Q120 ；T值传递参数#define DArg Q121 ；D值传递参数#define IArg Q109 ；I值传递参数使用G代码的PMAC程序OPEN PROG 1000 CLEARRAPID RETURN ；G00 快速子程序;... ；其他子程序N78000 ；G78内部螺纹加工READ(X,Y,Z,R,P,T,D,I) ；调用程序参数；将传输的值转换为关键参数CenterX=XArgCenterY=YArgBottomZ=ZArgPitch=PArgNumOfThreads=TArgThreadDepth=DArgDepthIncr=IArg；开始参数化进程RAPID ；快速模式开始ABS ；所有轴均为绝对模式X(CenterX) Y(CenterY) Z(RetractZ) C0 ；到达孔上方StartZ=BottomZ-Pitch/10Z(StartZ) ；Z运动至切削开始的坐标ToolCenterRad=InsideRad+DepthIncr-ToolLengthX(ToolCenterRad) ；刀具中心到达期望的运动半径; Loop once for each depth of cut；循环执行多个回合，直到到达期望切削深度FRAX(X,Y,Z) ；矢量速度包含的轴WHILE (ToolCenterRad+ToolLength<InsideRad+ThreadDepth)ThreadNum=0WHILE (ThreadNum<NumOfThreads+1)CIRCLE2 ；逆时针圆弧模式F(CutSpeed*InsideRad/(InsideRad-ToolLength))INC(Z,C) ；这些轴采用增量模式I(-ToolCenterRad) Z(Pitch) C360 ；X,Y运动一个完整圆弧，Z轴运动一个螺距，C轴旋转360°ThreadNum=ThreadNum+1 ；螺纹数增量计数ENDWHILERAPID ；快速开始下一个ABS(Z) ；绝对模式X(InsideRad-DepthIncr-ToolLength) ；清除孔内部Z(StartZ) ；Z运动至切削开始的坐标ToolCenterRad=ToolCenterRad+DepthIncr ；进入下一回合X(ToolCenterRad) ；增加切削深度ENDWHILEX(CenterX) Y(CenterY) Z(RetractZ) ；回到原位RETURNCLOSE调用部分程序实例OPEN PROG 50 CLEARG00 X0 Y0G78 X1000 Y200 Z50 R80 P5 T10 D3 I0.2G78 X1000 Y1000 Z50 R80 P5 T10 D3 I0.2G78 X2000 Y1000 Z50 R80 P5 T10 D3 I0.2G78 X2000 Y200 Z50 R80 P5 T10 D3 I0.2G78 X1200 Y400 Z50 R50 P2.5 T20 D2 I0.2G78 X1200 Y800 Z50 R50 P2.5 T20 D2 I0.2G78 X1800 Y800 Z50 R50 P2.5 T20 D2 I0.2G78 X1800 Y400 Z50 R50 P2.5 T20 D2 I0.2G00 X0 Y0CLOSEHelical Interpolation ExampleIn Turbo PMAC controllers, helical interpolation is simply an extension of the standard circular interpolation mode. Axes that are not circularly interpolated are automatically linearly interpolated in a coordinated fashion. If the axis is perpendicular to the plane of the circle, the result will be a helix. If the axis is a rotary axis turning around an axis perpendicular to the circular, the tool can rotate to stay at a fixed angle (e.g. tangent or normal) with regard to the path. For example, to do a full circle in the XY plane about the origin starting from the point {X=10,Y=0} the following commands could be used:NORMAL K-1 ; Specify XY plane w/ Z-vectorCIRCLE2 ; CCW circle modeABS ; Specify end points by location INC(R) ; Specify center by distanceX10 Y0 I-10 ; Circle move commandIf an axis is not explicitly commanded in a move, Turbo PMAC assumes the end position for the axis is the same as the start position. In circular interpolation, if none of the coordinates in the plane of the circle are specified, Turbo PMAC will execute a full circle. So the command for the above full-circle move could be shortened to:I-10To add a Z-axis move to Z=1 and a C-axis rotary move to 360 degrees, the command could be extended to:X10 Y0 I-10 Z1 C360Since this is a full-circle move, the move command could be simplified to:I-10 Z1 C360Application ExampleSometimes an inside thread will need to be cut that is too big to be tapped. These threads need to be cut with a single-point tool that can move in all three Cartesian coordinates and rotate to keep perpendicular to the cut surface. The Cartesian axes perform helical interpolation, and the rotary axis moves at constant velocity.To cut the thread to full depth, the program executes a series of passes, each pass at a slightly greater depth into the material. A pass is a series of full-circle helical moves, one for each thread specified. In between passes, RAPID-mode moves prepare for the next pass.Each CIRCLE-mode move creates a full circle in the XY-plane, with a Z-move distance of one pitch of the thread, and a 360-degree rotation of the C-axis. The programmed speed (F) is the vector velocity of the tool center in XYZ-space, because all three axes are commanded to be involved in the vector calculations with the FRAX(X,Y,Z) command (this is the default). This speed is derived in the program from the specified cut speed, because the tool center will move more slowly than the cutting tip. It would be possible to use tool (cutter) radius compensation in this example, but here the compensation is done explicitly in the program.The following diagram shows a top view and a side cross-sectional view of the operation.The following setup and programs can be used to implement this strategy.; Set up coordinate system&1 ; Address Coordinate System 1#1->400X ; X in mm, 2.5-um resolution#2->400Y ; Y in mm, 2.5-um resolution#3->400Z ; Z in mm, 2.5-um resolution#4->100C ; C in deg, 0.01-deg resolutionI428=36000 ; #4 (C) rollover at 36K countsI5113=10 ; CS1 exact circle calcs every 10ms I5190=60000 ; CS1 speeds in mm/min (60K msec); Substitutions and definitions#define CenterX Q500 ; X-coord of hole center#define CenterY Q501 ; Y-coord of hole center#define RetractZ Q502 ; Z-coord of tool-up position#define StartZ Q503 ; Z-coord of cut start#define BottomZ Q504 ; Z-coord of bottom of hole#define Pitch Q505 ; Thread pitch in user units#define ToolCenterRad Q506 ; Radius of motion#define InsideRad Q507 ; Radius of unthreaded hole#define DepthIncr Q508 ; Depth of cut each pass#define ToolLength Q509 ; From tool center to cut tip#define ThreadDepth Q510 ; Full depth of cut#define ThreadNum Q511 ; Counter for threads cut#define NumOfThreads Q512 ; Total number specified#define CutSpeed Q513 ; Tool-tip cutting speed; Set system constantsRetractZ=450 ; 450 mm above baseToolLength=25 ; 25 mm from center to cut tip; Set cut parametersCenterX=-220 ; In mm, from originCenterY=135 ; In mm, from originBottomZ=20 ; In mm, from originPitch=10 ; In mm, thread to threadInsideRad=55 ; In mm, from hole centerDepthIncr=0.2 ; In mm, pass to passToolLength=25 ; In mm, from tool center ThreadDepth=8.0 ; In mm, from uncut surface NumOfThreads=10 ; Number of full turnsCutSpeed=80 ; In mm/minOPEN PROG 60 CLEARRAPID ; Fast to start of cutABS ; All axes absoluteX(CenterX) Y(CenterY) Z(RetractZ) C0 ; Move over holeStartZ=BottomZ-Pitch/10Z(StartZ) ; Descend below bottom ToolCenterRad=InsideRad+DepthIncr-ToolLengthX(ToolCenterRad) ; Move to radiusFRAX(X,Y,Z) ; Axes in vector speed calcs ; Loop once for each depth of cut plus extra to enter and exit part WHILE (ToolCenterRad+ToolLength<InsideRad+ThreadDepth)ThreadNum=0; Loop once for each threWHILE (ThreadNum<NumOfThreads+1)CIRCLE2 ; CCW circle modeF(CutSpeed*InsideRad/(InsideRad-ToolLength))INC(Z,C) ; These axes incrementalI(-ToolCenterRad) Z(Pitch) C360 ; 1 helical rotationThreadNum=ThreadNum+1 ; Increment counterENDWHILERAPID ; Fast to start of nextABS(Z) ; To command by positionX(InsideRad-DepthIncr-ToolLength) ; To clear inside of holeZ(StartZ) ; Descend below bottomToolCenterRad=ToolCenterRad+DepthIncr ; For next cut passX(ToolCenterRad) ; Move to new cut depth ENDWHILEX(CenterX) Y(CenterY) Z(RetractZ) ; Retract toolCLOSEExecuting As Parameterized G-Code SubroutineOften an operation such as threading a hole is a subroutine in the overall programmed sequence. In machine-tool “G-code” style programs, this type of operation is typically considered a “canned cycle”, called from the part program with a series of parameters each specified as the numerical value following a particular letter. In this example, we will call the subroutine with the G78 code followed by 8 arguments, in the following style:G78 X Y Z R P T D Iwhere:the X-value is the X-coordinate of the center of the hole;the Y-value is the Y-coordinate of the center of the hole;the Z-value is the Z-coordinate of the bottom of the holethe R-value is the inside radius of the wholethe P-value is the pitch of the threadthe T-value is the number of threadsthe D-value is the thread depththe I-value is the depth incrementIn Turbo PMAC, G-code subroutines are implemented in PROG 1000, with the start of each subroutine having a line label number 1000 times the G-code number. So the G78 subroutine will start at label N78000 of PROG 1000.; Additional substitutions and definitions#define XArg Q124 ; Variable for passing X value#define YArg Q125 ; Variable for passing Y value#define ZArg Q126 ; Variable for passing Z value#define RArg Q118 ; Variable for passing R value#define PArg Q116 ; Variable for passing P value#define TArg Q120 ; Variable for passing T value#define DArg Q121 ; Variable for passing D value#define IArg Q109 ; Variable for passing I value; PMAC program to implement G-code subroutinesOPEN PROG 1000 CLEARRAPID RETURN ; G00 Rapid subroutine;... ; Other subroutines hereN78000 ; G78 Inside threading routine READ(X,Y,Z,R,P,T,D,I) ; Get params from part prog; Transfer passed values to key parametersCenterX=XArgCenterY=YArgBottomZ=ZArgPitch=PArgNumOfThreads=TArgThreadDepth=DArgDepthIncr=IArg; Start parameterized sequenceRAPID ; Fast to start of cutABS ; All axes absoluteX(CenterX) Y(CenterY) Z(RetractZ) C0 ; Move over holeStartZ=BottomZ-Pitch/10Z(StartZ) ; Descend below bottom ；ToolCenterRad=InsideRad+DepthIncr-ToolLengthX(ToolCenterRad) ; Move to radius; Loop once for each depth of cutFRAX(X,Y,Z) ; Axes in vector speed calcs WHILE (ToolCenterRad+ToolLength<InsideRad+ThreadDepth)ThreadNum=0; Loop once for each threadWHILE (ThreadNum<NumOfThreads+1)CIRCLE2 ; CCW circle modeF(CutSpeed*InsideRad/(InsideRad-ToolLength))INC(Z,C) ; These axes incremental I(-ToolCenterRad) Z(Pitch) C360 ; 1 helical rotationThreadNum=ThreadNum+1 ; Increment counterENDWHILERAPID ; Fast to start of next ABS(Z) ; To command by position X(InsideRad-DepthIncr-ToolLength) ; To clear inside of hole Z(StartZ) ; Descend below bottom ； ToolCenterRad=ToolCenterRad+DepthIncr ; For next cut passX(ToolCenterRad) ; Move to new cut depth ENDWHILEX(CenterX) Y(CenterY) Z(RetractZ) ; Retract toolRETURN;... ; Other subroutines here CLOSE; Sample calling part program; This program threads four large holes in a rectangular pattern; and four smaller holes in a smaller rectangleOPEN PROG 50 CLEARG00 X0 Y0G78 X1000 Y200 Z50 R80 P5 T10 D3 I0.2G78 X1000 Y1000 Z50 R80 P5 T10 D3 I0.2G78 X2000 Y1000 Z50 R80 P5 T10 D3 I0.2G78 X2000 Y200 Z50 R80 P5 T10 D3 I0.2G78 X1200 Y400 Z50 R50 P2.5 T20 D2 I0.2G78 X1200 Y800 Z50 R50 P2.5 T20 D2 I0.2G78 X1800 Y800 Z50 R50 P2.5 T20 D2 I0.2G78 X1800 Y400 Z50 R50 P2.5 T20 D2 I0.2G00 X0 Y0CLOSE。