CNC车床编程设计教学ppt课件

第二章車床程式設計,2-1基本機能簡介。2-2參考點及座標系統設定。2-3絕對座標與增量座標。2-4直徑指令與半徑指令程式。2-5輸入單位系統之選擇。2-6快速定位（G00）,1,第二章車床程式設計(續),2-7直線切削（G01）2-8原點復歸（G28）2-9圓弧切削（G02、G03）2-10暫停指令（G04）2-11單一固定切削循環（G90、G94）,2,第二章車床程式設計(續),2-12螺紋切削（G92）2-13複合固定切削循環（G70G76）,3,2-1基本機能簡介,電腦數值控制車床之程式是利用各種英文字母、數值、符號.等組成。機能指令,並歸類為六大類:G機能(準備機能：G00G99)M機能(輔助機能：M00M99)T機能(刀具機能)S機能(主軸轉速機能or切削機能),4,2-1基本機能簡介,F機能(進給機能)N機能(程式序號機能),5,各種G碼代表之意義及功能,G00：快速定位G01：直線插位(切削進給)G02：圓弧插位(順時針)G03：圓弧插位(逆時針)G04：暫停G20：英制資料輸入G21：公制資料輸入,6,各種G碼代表之意義及功能,G27：原點復歸檢查G28：原點復歸G32：螺紋切削G40：刀鼻半徑補正取消G41：刀鼻半徑偏左補正G42：刀鼻半徑偏右補正G50：最大主軸轉速設定,7,各種G碼代表之意義及功能,G70：精車切削循環G71：軸向複合形固定切削循環G72：端面複合形固定切削循環G73：輪廓複合形固定切削循環G74：端面（Z軸向）溝槽切削循環G75：軸向（X軸向）溝槽切削循環G76：螺紋複合形固定切削循環,8,各種G碼代表之意義及功能,G90：軸向固定切削循環G92：螺紋固定切削循環G94：端面固定切削循環G96：周速一定控制(切削速度設定)G97：主軸固定轉速設定（rpm）G98：每分鐘進給率（mm/min）G99：每轉進給率（mm/rev）,9,M機能又稱為輔助機能,M00：程式停止M01：選擇性程式停止M02：程式結束M03：主軸正轉CWM04：主軸反轉CCWM05：主軸停止,10,M機能又稱為輔助機能,M08：冷卻液開啟ONM09：冷卻液關閉OFFM30：程式結束,記憶還原M98：呼叫副程式M99：副程式結束,11,T機能(刀具機能),刀具機能是由T位址字元後面接續4個數字號碼所組成。前兩位數字群為刀塔上之刀具編號。後兩位數字群則是刀具之補正編號。刀具機能在使用時須將刀具號碼和補正號碼同時使用。程式中若使用00補正號碼時,代表刀具補正取消。,12,刀具機能補正範例,T0303:前兩碼03代表刀具號碼,後兩碼03代表補正號碼。T0514:前兩碼05代表刀具號碼,後兩碼14代表補正號碼。T0900:前兩碼09代表刀具號碼,後兩碼00代表補正號碼取消。,13,車床刀具資料：幾何【G】補正表,14,車床刀具資料：磨耗【W】補正表,15,S機能(主軸轉速機能),(一)固定切削速度設定(G96S200)EX：G96S200M03:切削速度為200(m/min)主軸正轉。【V=DN/1000】(二)最高主軸轉速設定(G50S2500)程式。EX：G5OS2500:最高轉速設定為2500rpm。,16,S機能(主軸轉速機能),(三)固定主軸轉速設定(G97S2000)通常可應用於鑽孔、切槽、螺紋切削。EX：G97S2000:主軸固定轉速為2000rpm,17,F機能又稱進給機能,刀具運動方式可分為兩種：快速運動：是執行刀具快速移動定位,須由快速定位機能指令G00執行,並可在機器操作面板上利用快速進給率轉鈕(F0、25%、50%、100%)予以調整。切削進給：則是在程式執行實際切削運動時(G01、G02、G03)用於指令其切削時之進給率。,18,F機能又稱進給機能,進給率方式可分為兩種：每分鐘進給率(mm/min)【G98】每轉進給率(mm/rev)【G99】車削加工則用每轉進給率(mm/rev)。銑削加工則用每分鐘進給率(mm/min)。,19,進給率方式可分為兩種每分鐘進給率(mm/min)【G98】每轉進給率(mm/rev)【G99】,20,N機能又稱程式序號機能,位址字元N及正整數組成(N0001N9999)程式序號一般為程式單節的第一個字語，程式之每一單節均須編寫程式序號。現今CNC控制器中則無須再編寫程式序號。通常只在程式執行特定控制迴路時予以使用(例：副程式指令、循環機能指令.等)。,21,2-2參考點設定,參考點(Referencecoordinates)：(1)機械參考點(Machinereferencepoint)稱為機械原點,它是機械上的一個固定的參考點。機械原點可作下列之用途:(a)作為刀具之交換點。(b)作為其他座標點之參考點。(c)機械開機後初始座標設定。,22,2-2參考點設定,(2)程式參考點(Programreferencepoints)：程式參考點又稱程式原點,它是工件上所有轉折點座標值之基準點,此點必須在編寫程式時加以選定。,23,圖4-1CNC車床之參考點位置,24,圖4-2座標系統之設定,25,程式原點設定【左邊】,26,程式原點設定【右邊】,27,2-3絕對座標與增量座標,座標之表示方式有兩種：絕對座標系統(Absolutepositioning)所謂絕對座標就是將程式原點設為永遠之座標零點,程式中之所有座標點均對該點設定之。增量座標系統(Incrementalpositioning)所謂增量座標則是程式中之座標點,均以其前一點為座標零點而設定之。,28,圖4-3絕對座標及增量座標工作圖,29,絕對座標：程式範例,O6001(程式檔名)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X65.0Z5.0(快速移到指定位置)X30.0G01Z0F0.2X45.0Z-20.0Z-40.0X65.0G00G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),30,增量座標：程式範例,O6002(程式檔名)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X65.0Z5.0X30.0G01Z0F0.2U15.0W-20.0W-20.0U17.5G00G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),31,2-4直徑指令與半徑指令程式,編寫程式時,其X方向的尺寸標示方式可分為兩種：直徑指令(Diameterprogramming)半徑指令(radiusprogramming)圓柱形工件其X方向的尺寸則應以直徑值表示。,32,2-5輸入單位系統之選擇,G20:英制單位系統G21:公制單位系統通常CNC車床之使用單位為公制系統,以被設定為公制單位系統(G21)。若該程式輸入之資料為英制單位時,則需在程式之開頭編寫(G20)之指令。,33,2-6快速定位（G00）,【指令格式】G00XZ；(絕對座標模式)G00UW；(增量座標模式)G00之XZ或UW是代表位移目標之指定位置。EX：G00X65.0Z5.0,34,圖4-5G00之運動路徑(一),35,圖4-6G00之運動路徑(二),36,2-7直線切削（G01）,【指令格式】G0lXZF(絕對座標模式)G0lUWF(增量座標模式)G0l後面之XZ或UW是代表刀具切削之目標指定位置。F則代表切削之進給率：單位為公厘/每轉(mm/rev)。EX：G01X65.0Z5.0F0.2mm/rev。,37,圖4-8直線切削之路徑,38,圖4-8軸向直線切削範例(P1),O6005(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X45.0Z1.0(快速移到指定位置)G01Z-40.0F0.3(直線切削),39,圖4-8軸向直線切削範例(P2),X52.0(直線切削)X65.0G00G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),40,圖4-7端面切削之路徑,41,圖4-7端面直線切削範例(P1),O6006(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X52.0Z-1.0(快速移到指定位置)G01X-1.8F0.2(直線切削),42,圖4-7端面直線切削範例(P2),Z5.0(直線切削)G00X60.0Z10.0(快速移至目標位置)G00G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),43,2-7直線切削（G01）,直線切削(G01)一般可車削：端面車削外徑車削錐度車削切槽車削鑚孔車削搪孔車削,44,圖4-9錐度之定義,45,圖4-11錐度車削之路徑,46,圖4-11錐度車削範例(P1),O6007(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X27.0Z2.0(快速移到指定位置)G01Z0F0.2(直線切削),47,圖4-11錐度車削範例(P2),X35.0Z-40.0(錐度切削)Z-50.0(直線切削)X55.0(直線切削)G00X60.0Z10.0(快速移至目標位置)G00G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),48,2-8原點復歸（G28）,原點復歸時先快速位移至指定位置(G28XZorG28U0W0座標值)，以自動方式回機械原點。因此G28指令之座標點可謂回機械原點前之中間點。EX：G28X65.0Z-20.0EX：G28U5.0W5.0EX：G28U0W0,49,以絕對座標模式自動原點復歸範例：,EX：G28X65.0Z-20.0【圖4-12】,50,以增量座標模式自動原點復歸範例：,EX：G28U5.0W5.0【圖4-13】,51,以增量座標模式，且增量值為零，自動原點復歸範例：,EX：G28U0W0【圖4-14】,52,圖4-15直線切削實作練習,53,圖4-15直線切削程式設計,O6014(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(外粗刀號碼及補正代號)G96S200M03(設定切削速度)G00X70.0Z5.0(快速移到指定位置)G94X-1.8Z2.0F0.3Z1.0,54,Z0G00X70.0Z3.0G71U2.0R1.0G71P10Q20U0.4W0.2F0.3N10G00G42X20.0G01X30.0Z-2.0F0.1Z-22.0X42.0Z-42.0X51.0,55,Z-55.0X58.0Z-70.0X65.0Z-72.0N20X70.0G00G40G28U0W0M05G50S3000T0303(外精刀號碼及補正代號),56,G96S240M03(設定切削速度)G00X70.0Z3.0(快速移至目標位置)G70P10Q20(精車指令)G00G40G28U0W0M05(自動回機械原點)M30(程式結束、程式還原),57,圓弧切削機能指令,圓弧切削機能指令時,程式中須提供五項完整之資料,包括：(1)圓弧之起點座標(XZ)(2)圓弧切削之方向(G02、G03)(3)圓弧切削之終點座標(XZ)(4)圓弧之半徑值或圓弧中心點位置(RorI、J)(5)圓弧切削進給率(F),58,圓弧之半徑值(R)方法,【指令格式】G02XZRF(絕對座標模式)順G02UWRF(增量座標模式)順G03XZRF(絕對座標模式)逆G03UWRF(增量座標模式)逆,59,定義圓弧規格時可使用兩種方式,圓弧之半徑值(R)方法：其中以R標示方式較為簡便，數控車床車削圓弧較佳。圓弧之中心點位置(I、K)方法：用來切削全圓弧較佳。,60,圓弧切削R值有正.負號區分,其R值有正.負號之分：正.負值之判斷依據是以圓弧起點至圓弧終點之夾角：詳細規定如下：(夾角)=0180。(R值為正)(夾角)=181359(R值為負)(夾角)=360。(無法以R標示方式,須以I.K標示方式),61,圖4-19相同值有兩種圓弧形式,62,圖4-20順時針(G02)圓弧切削之範例,63,圖4-21逆時針(G03)圓弧切削之範例,64,圖4-26圓弧切削練習【G02.G03】,65,圖4-26直線及圓弧切削之程式,O6019(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(外粗車刀號碼及補正代號)G96S200M03(設定切削速度)G00X70.0Z3.0M08(快速移到指定位置)G94X-1.8Z2.0F0.3(車端面)Z1.0,66,Z0G71U2.0R1.0G71P10Q20U0.4W0.2F0.3N10G00G42X16.0G01X23.985Z-1.0F0.1Z-10.0X24.98G03X40.98Z-18.0R8.0G01Z-42.0,67,X50.98Z-66.0G02X62.98Z-72.0R6.0G01X65.0Z-74.0N20X70.0G00G40G28U0W0M05G50S3000,68,T0303(外精刀號碼及補正代號)G96S240M03(設定切削速度)G00X70.0Z3.0(快速移至目標位置)G70P10Q20(精車指令)G00G40G28U0W0M05(自動回機械原點)M09M30(程式結束、程式還原),69,圖4-30圓弧切削練習【內徑車削】,70,圖4-30直線及圓弧切削【內徑車削】,O6025(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0707(鑚孔刀具號碼及補正代號)G97S800M03(設定切削速度)G00X0Z8.0M08(快速移到指定位置)G74R1.0G74Z-52.0Q3000F0.05,71,G00G28U0W0M05G50S3000T0101G96S200M03G00X70.0Z5.0G94X18.0Z2.0F0.3Z1.0Z0,72,G00G28U0W0M05G50S3000T0606G96S200M03G00X18.0Z3.0G71U2.0R1.0G71P10Q20U-0.4W0.2F0.3N10G00G41X59.04G01X51.04Z-1.0F0.1,73,Z-6.0X41.04Z-32.0G03X29.04Z-38.0R6.0G01X24.04Z-48.0N20X20.0G00G40G28U0W0M09,74,G50S3000T0808G96S240M03G00X18.0Z3.0G70P10Q20G00G40G28U0W0M05M09M30,75,2-10暫停指令（G04）,電腦數值控制車床之暫停指令（G04）,通常用於切槽或鑚孔加工。【指令格式】G04X(可有小數點)(X1.0=1Sec)G04U(可有小數點)(U1.0=1Sec)G04P(不可有小數點)(P1000=1Sec)指令單位為秒(Sec),76,2-11單一固定切削循環（G90）,軸向固定切削循環（G90）可分為(1)直線切削模式：【指令格式】G90XZF(絕對座標模式)G90UWF(增量座標模式)刀具路徑：ABCDA循環,77,圖4-36外形固定切削循環(直線切削模式),78,圖4-41固定切削循環範例圖(直線切削),79,圖4-41固定切削循環範例程式(P1),O6026(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0303(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X67.0Z2.0M08(快速移到指定位置)G90X60.0Z-40.0F0.3(固定切削循環指令),80,X55.0(固定切削循環指令)X50.0(固定切削循環指令)X45.0(固定切削循環指令)G00G28U0W0M05(自動回機械原點)M09M30(程式結束、程式還原),81,2-11單一固定切削循環（G94）,端面固定切削循環（G94）可分為(1)直線切削模式：【指令格式】G94XZF(絕對座標模式)G94UWF(增量座標模式)刀具路徑：ABCDA循環,82,圖4-43端面固定切削循環(直線切削模式),83,圖4-48端面切削循環範例圖(直線切削),84,圖4-48端面切削循環範例程式(P1),O6029(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S200M03(設定切削速度)G00X95.0Z2.0M08(快速移到指定位置),85,圖4-48端面切削循環範例程式(P2),G94X20.0Z-2.0F0.3(端面切削循環)Z-4.0(端面切削循環)Z-6.0(端面切削循環)G00G28U0W0M05(自動回機械原點)M09M30(程式結束、程式還原),86,2-12螺紋切削公制螺紋,87,加工不同型式螺紋之樣品圖：（P1）,88,加工不同型式螺紋之樣品圖：（P2）,89,(1)主軸轉速之決定,90,(2)計算不完整螺紋距離1及2,91,(3)計算螺紋之牙深及規劃切削次數,92,(4)規劃螺紋每刀切削量及切削次數,93,(5)決定進刀方式及退刀方式,94,螺紋切削（G92）,【指令格式】【直線螺紋切削循環】G92XZF(E)(絕對座標模式)G92UWF(E)(增量座標模式)X(U),Z(W)螺紋切削終點之座標值F：螺紋之導程值E：通常使用英制系統之螺紋(可用至小數點四位),95,圖4-66直線螺紋之切削路徑,刀具路徑：ABCCDA循環,96,圖4-68：以G92車削平行螺紋之範例,97,圖4-68：以G92車削平行螺紋之程式,O6035(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0404(刀具號碼及補正代號)G97S1000M03(設定切削轉速rpm)G00X35.0Z8.0M08(快速到指定位置)G92X29.52Z-52.0F2.0(第一次車削X值),98,X29.08(第二次車削X值)X28.70(第三次車削X值)X28.38(第四次車削X值)X28.10(第五次車削X值)X27.90(第六次車削X值)X27.74(第七次車削X值)X27.60(第八次車削X值)X27.50(第九次車削X值)X27.40(第十次車削X值)G00G28U0W0M05(自動回機械原點)M09(冷卻劑off)M30(程式結束、程式還原),99,2-13複合固定切削循環（G70G76）,CNC可在車削過程中,自動產生一系列之切削路徑,完成工件之輪廓切削。提高程式設計之效率,並降低程式編寫之難度,為了達成此任務,在CNC車床控制器內建構了一群複合固定切削循環機能。在編寫程式時,只要給予工件內.外形(直線、錐度、圓弧等之輪廓),刀具便能依指示逐次切除欲車削之部位。,100,複合形固定切削循環(G70G76),G70：精車切削循環(配合G71.G72.G73)G71：軸向複合形固定切削循環G72：端面複合形固定切削循環G73：輪廓複合形固定切削循環G74：端面(Z軸向)溝槽切削循環G75：軸向(X軸向)溝槽切削循環G76：螺紋自動切削循環,101,G71：軸向複合形固定切削循環,【指令格式】G71U(d)R(e)G71P(ns)Q(nf)U(u)W(w)F(f)G71指令只被應用於工件之粗車再配合精車切削循環指令(G70)方可達成任務。其詳細切削路徑如圖4.75所示。,102,【格式說明】,103,圖4-74G71指令中UW之正負符號判斷,104,圖4-75G71指令之切削路徑,圖示中d為每次之切削深度.U/2及w為精車之預留量【第一次路徑C1234】,105,G70：精車切削循環(配合G71.G72.G73),【指令格式】G70P(ns)Q(nf)【格式說明】ns：開始循環之單節順序號碼（精車）nf：最後循環之單節順序號碼（精車）,106,圖4-76G71.G70複合形固定切削循環練習,107,圖4-76：以G71.G70車削之程式(P1),O6041(程式檔名)G00G28U0W0(自動回機械原點)G50S2500(設定主軸最高轉速)T0101(刀具號碼及補正代號)G96S180M03(設定切削速度)G00X70.0Z3.0M08(快速到指定位置)G94X-1.8Z2.0F0.2(車削端面)Z1.0,108,圖4-76：以G71.G70車削之程式(P2),Z0G71U2.0R1.0G71P10Q20U0.4W0.2F0.3N10G00G42X16.0G01X25.0Z-1.5F0.1Z-20.0X33.0X38.0Z-45.0,109,圖4-76：以G71.G70車削之程式(P3),Z-50.0X46.0G02X58.0Z-56.0R6.0G01Z-75.0N20X70.0G00G28U0W0M05G50S3000T0303,110,圖4-76：以G71.G70車削之程式(P4),G96S200M03G00X70.0Z3.0G70P10Q20(精車指令)G00G40G28U0W0M05M09M30,111,G74：端面(Z軸向)溝槽切削循環,【指令格式】G74R(e)G74X(U)Z(W)P(i)Q(k)R(d)F(f),112,【格式說明】,113,圖4-82G74端面溝槽切削循環之切削路徑,114,圖4-84G74鑚孔循環練習範例圖,115,圖4-84G74鑚孔循環練習程式(P1),O6047(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0606(鑚頭刀具號碼及補正代號)G97S800M03(設定切削轉速rpm)G00X0Z3.0M08(快速到指定位置)G74R1.0G74Z-35.0Q5000F0.08,116,圖4-84G74鑚孔循環練習程式(P2),G00G28U0W0M05M09M30,117,G75：軸向(X軸向)溝槽切削循環,【指令格式】G75R(e)G75X(U)Z(W)P(i)Q(k)R(d)F(f),118,【格式說明】,119,【格式說明】,120,圖4-85G75軸向(X軸向)溝槽切削循環之切削路徑,121,圖4-86G75軸向(X軸向)溝槽切削循環機能指令練習圖,122,圖4-86G75外徑溝槽切削循環程式(P1),O6048(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T1010(切槽刀具號碼及補正代號)G97S600M03(設定切削轉速)G00X70.0Z-25.0M08(快速到指定位置)G75R1.0G75X40.0Z-40.0P5000Q4000F0.08,123,圖4-86G75外徑溝槽切削循環程式(P2),G00G28U0W0M05M09M30,124,圖4-133G75外徑溝槽切削循環圖,125,圖4-133使用G75車削指令範例程式,O6049(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T1010(切槽刀刀具號碼及補正代號)G97S800M03(設定切削轉速)G00X57.0Z-12.0M08(快速到指定位置)G75R1.0G75X48.0Z-60.0P2000Q12000F0.05G00G28U0W0M05M09M30,126,G76：螺紋自動切削循環,【指令格式】G76P(m)(r)(a)Q(dmin)R(d)G76X(U)Z(W)R(i)P(k)Q(d)F(L)m：精車次數。r：倒角長度之倍數(以導程計算)。a：螺紋之螺紋角。,127,【格式說明】,128,圖4-88G76螺紋車削之進刀方式與深度示意圖,129,圖4-89以G76機能車削螺紋之範例圖,130,圖4-89G76機能車削螺紋程式(P1),O6050(程式檔名)G00G28U0W0(自動回機械原點)G50S3000(設定主軸最高轉速)T0404(外徑牙刀刀具號碼及補正代號)G97S1200M03(設定切削轉速rpm)G00X35.0Z8.0M08(快速到指定位置)G76P021060Q40R0.04(G76螺紋車削)G76X27.4Z-52.0P1300Q450F2.0,131,圖4-89G76機能車削螺紋程式(P2),G00G28U0W0M09M05M30(1)精車二次,倒角量=導程,螺紋為60。(2)粗車最小切削量0.04mm(3)精車預留量0.04mm(4)螺紋終點座標為(X27.4，Z-52.0)(5)螺紋之牙深為1.3mm，P=1300(6)第一刀之切削深度為0.45mm(半徑).Q=450(7)螺紋之導程為2mm，F=2.0,132,4-15刀鼻半徑補正（G40G42）,133,圖4-120刀鼻半徑補正機能指令之應用,134,刀鼻半徑補正機能指令G41.G42,135,刀鼻半徑補正機能指令G41.G42,136,圖4-104刀具之假想刀尖,137,圖4-105未作刀鼻半徑補正圖,138,圖4-106端面及平行外徑不須刀鼻半徑補正,139,圖4-107.108刀鼻半徑補正圖,140,圖4-112未考慮刀鼻半徑補正圖,141,圖4-113考慮刀鼻半徑補正圖,142,表4-20刀鼻半徑補正輸入,143,圖4-121假想刀尖與刀鼻圓心之方向,144,假想刀尖與刀鼻圓心之方向,145,術科檢定題目(材料圖)(丙),146,術科檢定題目(第一題)(丙),A=92.0B=30.0C=24.0倒角為1x45,147,【第一題程式設計】,O9001G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03M08G00X66.0Z5.0G94X-1.8Z2.0F0.2Z1.0Z0.5Z0F0.1,148,G71U2.0R1.0G71P10Q20U0.3W0.1F0.2N10G00G42X10.85G01X24.85Z-2.0F0.1Z-24.0X27.97X29.97Z-25.0Z-30.0X37.637Z-53.0X46.02X48.02Z-54.0,149,Z-62.0G02X56.02Z-66.0R4.0G01X58.0N20X62.0Z-68.0G00G40G28U0W0G50S2000T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P10Q20G00G40G28U0W0,150,G50S2000T0404【外螺紋車刀：=60】G97S1200M03G00X30.0Z10.0G76P021060Q200R0.03G76X23.05Z-21.0P974Q300F1.5G00G28U0W0M05M09M30,151,術科檢定題目(第二題)(丙),A=46.0B=13.0C=1:6倒角為1x45,152,【第二題程式設計】,O9002G00G28U0W0G50S2000T0101【外粗車刀】G96S160M03M08G00X66.0Z5.0G94X-1.8Z2.0F0.2Z1.0Z0.5Z0F0.1,153,G71U2.0R1.0G71P10Q20U0.3W0.1F0.2N10G00G42X20.81G01X25.98Z-26.0F0.1Z-30.0X29.85Z-32.0Z-52.0X44.0X46.0Z-53.0Z-62.0G02X52.0Z-65.0R3.0,154,G01X58.0N20X62.0Z-67.0G00G40G28U0W0G50S2000T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P10Q20G00G40G28U0W0G50S2000,155,T0404【外螺紋車刀：=60】G97S1200M03G00X35.0Z-25.0G76P021060Q200R0.03G76X28.05Z-49.0P974Q300F1.5G00G28U0W0M09M05M30,156,術科檢定題目(第三題)(丙),A=46.0B=32.0C=19.0倒角為1x45,157,【第三題程式設計】,O9003G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03M08G00X66.0Z5.0G94X-1.8Z2.0F0.2Z1.0Z0.5Z0F0.1,158,G71U2.0R1.0G71P10Q20U0.3W0.1F0.2N10G00G42X0G01Z0F0.1G03X20.0Z-10.0R10.0G01Z-16.0X30.0X32.0Z-17.0Z-44.0G02X38.0Z-47.0R3.0G01X43.98,159,X45.98Z-48.0Z-66.0X58.0X62.0Z-68.0N20G00X66.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P10Q20,160,G00G40G28U0W0G50S2500T1010【外切槽車刀：W=3mm】G97S900M03G00X65.0Z5.0X35.0Z-29.0G75R1.0G75X25.95Z-35.P2000Q2000F0.05X66.0Z5.0G00G40G28U0W0M09M05M30,161,術科檢定題目(第四題)(丙),A=47.0B=22.0C=19.0倒角為1x45,162,【第四題程式設計】,O9004G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03M08G00X65.0Z5.0G94X28.0Z3.0F0.2X2.0Z1.0Z0F0.1,163,G00G28U0W0G50S2500T0606【內粗搪孔刀】G96S180M03G00X30.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X55.6G01X45.03Z-0.3F0.1Z-10.0X39.0,164,G02X37.0Z-11.0R1.0G01Z-29.0X33.0N20X30.0Z-30.5G00G40G28U0W0G50S2500T0808【內精搪孔刀】G96S200M03G00X30.0Z5.0G70P10Q20G00G40G28U0W0,165,G50S2500T0101【外粗車刀】G96S160M03G00X66.0Z5.0G71U2.0R1.0G71P30Q40U0.3W0.1F0.2N30G00G42X42.0G01X54.0Z-1.0F0.1Z-47.0X58.0G03X62.0Z-49.0R2.0,166,G01Z-63.0N40G00X66.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P30Q40G00G40G28U0W0G50S2500T1010【外切槽車刀：W=3mm】,167,G97S600M03G00X66.0Z5.0X60.0Z-25.0G75R1.0G75X46.95Z-34.0P2000Q2000F0.05G00X66.0Z5.0G00G28U0W0M09M05M30,168,術科檢定題目(第五題)(丙),A=90.0B=50.0C=15.0倒角為1x45,169,【第五題程式設計】,O9005G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03M08G00X65.0Z5.0G94X28.0Z3.0F0.2X2.0Z1.0Z0F0.1,170,G00G28U0W0G50S2500T0606【內粗搪孔刀】G96S180M03G00X30.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X56.63G01X46.03Z-0.3F0.1Z-12.91X40.0,171,G02X38.0Z-13.91R1.0G01Z-27.91X33.0N20X30.0Z-29.41G00G40G28U0W0G50S2500T0808【內精搪孔刀】G96S200M03G00X30.0Z5.0G70P10Q20G00G40G28U0W0,172,G50S2500T0101【外粗車刀】G96S160M03G00X66.0Z5.0G71U2.0R1.0G71P30Q40U0.3W0.1F0.2N30G00G42X53.5G01X56.975Z-30.0F0.1Z-43.0X60.0X62.0Z-44.0,173,Z-64.0N40G00X66.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P30Q40G00G40G28U0W0G50S2500T1010【外切槽車刀：W=3mm】,174,G97S600M03G00X66.0Z5.0X60.0Z-38.0G75R1.0G75X50.0Z-43.0P2000Q2000F0.05G00G28U0W0M09M05M30,175,術科檢定題目(第六題)(丙),A=45.0B=22.0C=14.0倒角為1x45,176,【第六題程式設計】,O9006G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03M08G00X65.0Z5.0G94X28.0Z3.0F0.2X2.0Z1.0Z0F0.1,177,G50S2500T0606【內粗搪孔刀】G96S180M03G00X30.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X52.63G01X42.03Z-0.3F0.1Z-14.09X37.1X36.5Z-14.39,178,Z-29.09X33.0N20X30.0Z-30.59G00G40G28U0W0G50S2500T0808【內精搪孔刀】G96S200M03G00X30.0Z5.0G70P10Q20G00G40G28U0W0G50S2500,179,T0101【外粗車刀】G96S160M03G00X66.0Z5.0G71U2.0R1.0G71P30Q40U0.3W0.1F0.2N30G00G42X40.85G01X54.85Z-2.0F0.1Z-45.0X60.0X62.0Z-46.0Z-64.0,180,N40G00X66.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P30Q40G00G40G28U0W0G50S2500T0404【外螺紋車刀：=60】G97S600M03,181,G00X66.0Z10.0G76P021060Q200R0.03G76X53.05Z-23.0P974Q300F1.5G00G28U0W0M09M05M30,182,術科檢定題目(材料圖)(乙),183,術科檢定題目(第一題)(乙),A=92.0B=28.0C=10.0D=16.0,184,【第一題搪孔端】程式解答,O9011G00G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0M08G94X26.0Z0.5F0.1Z0G00G28U0W0G50S2500,185,T0606【內粗搪孔刀】G96S180M03G00X26.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X39.826G01X38.02Z-13.06F0.1Z-28.06N20X26.0G00G40G28U0W0G50S2500,186,T0808【內精搪孔刀】G96S200M03G00X26.0Z5.0G70P10Q20G00G40G28U0W0G50S2500T0101【外粗車刀】G96S180M03G00X66.0Z5.0G71U2.0R1.0G71P30Q40U0.3W0.1F0.2,187,N30G00G42X45.985G01X57.985Z-1.0F0.1Z-32.0X60.0X62.0Z-33.0Z-41.0N40X66.0G00G28U0W0G50S2500T0303【外精車刀】G96S200M03,188,G00X66.0Z5.0G70P30Q40G00G40G28U0W0G50S2500T0202【外圓鼻車刀】R=16mmG96S180M03G00X90.0Z5.0G42G01X88.0Z-3.0F0.2G02X88.0Z-35.0R16.0G40G01X90.0Z5.0G42G01X86.0Z-3.0,189,G02X86.0Z-35.0R16.0G40G01X90.0Z5.0G42G01X85.0Z-3.0G02X85.0Z-35.0R16.0G40G01X90.0Z5.0G42G01X84.0Z-3.0F0.1G02X84.0Z-35.0R16.0G40G01X90.0Z5.0G00G28U0W0M09M05M30,190,【第一題車螺紋端】程式解答,O9012G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03G00X66.0Z5.0M08G94X-1.8Z2.0F0.2Z1.0Z0F0.1,191,G71U2.0R1.0G71P50Q60U0.3W0.1F0.2N50G00G42X15.82G01X29.82Z-2.0F0.1Z-22.0X35.385G03X35.985Z-22.30R0.3G01Z-34.0X42.0G03X62.0Z-44.0R10.0G01Z-55.0,192,N60X66.0G40G00G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P50Q60G00G40G28U0W0G50S2500T0404【外螺紋車刀：=60】G97S1200M03,193,G00X35.0Z10.0G76P021060Q200R0.03G76X27.4Z-18.0P1300Q300F2.0G00G28U0W0G50S2500T1010【外切槽車刀：W=3mm】G97S600M03G00X70.0Z-53.05G75R1.0G75X54.05Z-54.95P2000Q2000F0.05G01X70.0Z-55.6,194,X62.6X61.4Z-55.0X54.0G04P300G01Z-53.0G04P300G01X61.4X62.6Z-52.6G00X70.0Z5.0G28U0W0M09M05M30,195,術科檢定題目(第二題)(乙),A=36.0B=12.0C=52.0D=35.0,196,【第二題搪孔端】程式解答,O9021G00G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G94X26.0Z0.5F0.1Z0G00G28U0W0G50S2500T0606【內粗搪孔刀】,197,G96S180M03G00X28.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X52.6G01X42.0Z-0.3F0.1Z-12.045X35.62X35.02Z-12.345Z-30.0N20X28.0,198,G00G40G28U0W0G50S2500T0808【內精搪孔刀】G96S200M03G00X28.0Z5.0G70P10Q20G00G40G28U0W0G50S2500T0101【外粗車刀】G96S180M03G00X66.0Z5.0,199,G71U2.0R1.0G71P30Q40U0.3W0.1F0.2N30G00G42X45.985G01X57.985Z-1.0F0.1Z-32.0X60.0X62.0Z-33.0Z-45.0N40X66.0G00G40G28U0W0G50S2500,200,T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P30Q40G00G40G28U0W0G50S2500T1010【外切槽車刀：W=3mm】G97S600M03G00X66.0Z-30.05G75R1.0G75X52.05Z-31.95P2000Q2000F0.05,201,G00X66.0Z-32.0G01X52.0G04P300G01Z-30.0G04P300G01X57.4X58.6Z-29.4G00X66.0Z5.0G00G28U0W0M09M05M30,202,【第二題車螺紋端】程式解答,O9022G00G28U0W0G50S2500T0101【外粗車刀】G96S180M03G00X66.0Z5.0G94X-1.8Z2.0F0.2Z1.0Z0.5Z0F0.1,203,G71U2.0R1.0G71P50Q60U0.3W0.1F0.2N50G00G42X0G01Z0F0.1G03X20.0Z-10.0R10.0G01Z-12.0X25.82X29.82Z-14.0Z-30.0X34.0G03X36.0Z-31.0R1.0,204,G01Z-35.0X41.0Z-50.0X60.0X64.0Z-52.0N60X66.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G70P50Q60,205,G00G40G28U0W0G50S2500T0404【外螺紋車刀：=60】G97S1200M03G00X35.0Z-6.0G76P021060Q200R0.03G76X27.4Z-27.0P1300Q300F2.0G00G28U0W0M09M05M30,206,術科檢定題目(第三題)(乙),A=50.0B=32.0C=24.0D=15.0,207,【第三題搪孔端】程式解答,O9031G00G28U0W0G50S2500T0303【外精車刀】G96S200M03G00X66.0Z5.0G94X26.0Z0.5F0.1Z0G00G28U0W0M05G50S2500,208,T0606【內粗搪孔刀】G96S180M03G00X28.0Z5.0G71U1.5R1.0G71P10Q20U-0.3W0.1F0.2N10G00G41X47.0G01X43.0Z-15.0F0.1X37.6X37.0Z-15.3Z-28.0N20X28.0,209,G00G40G28U0W0M05G50S2500T0808【內精搪孔刀】G96S200M03G00X28.0Z5.0G70P10Q20G00G40G28U0W0M05G50S2500T0101【外粗車刀】G96S180M03G00X66.0Z5.0,210,G71U2.0R1.0G71P30Q40U0.3W0.1F0.2N30G00G42X45.985G01X57.985Z-1.0F0.1Z-32.0X60.0N40X66.0Z-35.0G00G40G28U0W0G50S2500T0303【外精車刀】G96S200M03,211,G0