Delcam软件在发动机加工中的运用

　　DELCAM公司的PowerMILL软件提供的缺省的后处理可以满足三维加工的要求。而在二维加工中，孔位加工（钻、扩、铰、攻丝和镗等）都以G81为主，其中攻丝时缺少节距和停留时间等参数。以FANUC为例，进行攻丝钻孔时，应用缺省的后处理，生成的G代码格式如下：

　　G81G99Z-167.R-95.F341

　　应用笔者开发的后处理程序所生成的代码如下：

　　G84G99Z-167.0R-95.0P300F2.0

　　针对上述情况，笔者分别为TOYODA、YEONGCHIN和TOSHIBA三种加工中心开发了PowerMILL软件孔位加工（钻、扩、铰、攻丝和镗等）的后处理程序，从而使所有的孔位加工功能得到充分的发挥，保证产品加工过程的工艺要求。

　　YEONGCHIN加工中心的后处理如下：

machinefanuc15m
#OriginaloptionbyFaw_DDEWLiGuangQuan
definewordNT
addressletter="T"
addresswidth=1
fieldwidth=2
notmodal
enddefine
definewordTS
addressletter="N"
addresswidth=1
fieldwidth=3
notmodal
enddefine
definewordTPN
addressletter="(TOOLPATH:*******"
addresswidth=20
fieldwidth=30
enddefine
defineformat(ID)
addressletter=":"
enddefine
defineformat(N)
notpermanent
enddefine
defineformat(G1)
leadingzeros=true
notmodal
enddefine
defineformat(F)
modal
decimalpoint=true
decimalplaces=2
trailingzeros=false
imperialformats=metricformats
enddefine
defineformat(HM1M2)
leadingzeros=true
enddefine
defineformat(P)
fieldwidth=3
metricformats
decimalpoint=false
decimalplaces=0
trailingzeros=true
imperialformats=metricformats
enddefine
definewordPF
addressletter="F"
fieldwidth=5
notmodal
metricformats
decimalpoint=true
decimalplaces=2
trailingzeros=false
imperialformats=metricformats
enddefine
defineformatall
tapeposition=0
enddefine　
wordorder=(+TPNNTTSPPFD)
definekeys
toolradius=D
cycledwell=P
dwellnotused
enddefine
definecodes
cycleretract=G699
linear=G11
compoff=G240
componleft=G241
componright=G242
enddefine
messageoutput=false
blockorder=true
toolresetcoordinates=3
integer51=4
integer69=2
incrementalcentre=false
integer34=0
integer35=1
integer36=0
integer37=1
defineblocktapestart
"%"
IDProgID
rapid;incrementaldata;G628;zcoord0
incrementaldata=C;G630;ycoord0;xcoord0
enddefine
defineblocktoolchangefirst
toolnumberToolNumber
changetool
if(NextTool<>0)
　　　 NTNextTool
endif
TSToolNumber
setswa
enddefine
defineblocktoolchange
if(word[30]=7orword[30]=8)
M29
endif
rapid;incrementaldata;G628;zcoord0
incrementaldata;G630;ycoord0;xcoord0
compensationoff;G149;G480=C
changetool
if(NextTool<>0)
　　　 NTNextTool
endif
TSToolNumber
setswa
enddefine
defineblockmoverapid
if(swa)
TPNToolPathName;")"
G259;absolutedata;rapid;G6;xcoord;
ycoord;zcoord;spindle;toollength;M1;M2
unsetswa
else
rapid;G6;xcoord;ycoord;zcoord;spindle;
toollength;M1;M2
endif
enddefine
defineblockmovelinear
linear;G2;xcoord;ycoord;zcoord;toolradius;
feedrate;M1;M2
enddefine
defineblockmovecircle
N;G1;G3;xcoord;ycoord;zcoord;keyi; keyj;keyk;feedrate
enddefine
defineblockcyclestart
if(cycle=1)
G4;cycleretract;xcoord;ycoord;
drillholedepth;clearplane;feedratePrat
endif
if(cycle=2orcycle=3orcycle=>5)
G4;cycleretract;xcoord;ycoord;drillholedepth;
clearplane;cycledwell;feedratePrat
endif
if(cycle=4)
G4;cycleretract;xcoord;ycoord;drillholedepth;
clearplane;cycledwell;
PF(Cycfed/ToolSpeed[ToolNum])
endif
enddefine
defineblockmovecycle
xcoord;ycoord;M1;M2
enddefine
defineblockmovetap
xcoord;ycoord;M1;M2
enddefine
defineblockcycleend
endofdrill
enddefine
defineblocktapeend
if(word[30]=7orword[30]=8)
M29
endif
rapid;incrementaldata;G628;zcoord0
rapid;incrementaldata=C;G628;ycoord0
G140;G249;G480=C
changetool
endoftape
enddefine
end