马上注册，结交更多同行朋友，交流，分享，学习。
您需要 登录 才可以下载或查看，没有帐号？注册
x
Linear moves线性移动G01
( Up-dated 13/08/2002 )
The normal minimum output format for a linear move is
G01 X... Y... Z... F...
where G01 ( or G1 ) is the code for linear.
X Y and Z are the absolute or incremental positions.
F is the feed rate
The spindle speed and tool length offset may also appear on a linear move, this is more likely with multi-axes moves.
Also cutter compensation codes could be set if required, this is also more likey with PowerMill 3.0 2D machining..
A define block move linear is very rarely defined in the source files..
比较常用的线性移动表达式为： G01 X... Y... Z... F... 这里G01(G1)是线性移动的代码，X Y Z是相对或者绝对坐标系下的数值，F表示进给速度。还有主轴转速或者刀长补正也可能出现在线性移动的表达式后面。或许半径补偿也会出现大多数是在PM里面的2D加工中
However, it is recomended that if the block is not set up in the Source Post Processor control file, the example below would be better defined in the option. . ( In very rare circumstances it has been found that possible errors could occur if not set up )
然而，我们建议如果原处理程序里面没有定义线性移动，那么下面的例子里面是比较好的定义方法。（如果没有定义，在很少的情况下会发生错误警报）
The option file " define block move linear " could look like this :-
define block move linear
N ; G1 ; G2 ; X ; Y ; Z ; D ; F ; M1 ; M2
end define
( G1 is the linear code ( output normally G1 ), G2 is the cutter compensation code ( normally G41 or G42 ), D is the tool radius offset, F is the feed rate,.and M1, M2 will be M function codes. [ For multi-axes options it would be prudent to add G6, S and H ]
在文件里面通常这样定义线性移动。
define block move linear
N ; G1 ; G2 ; X ; Y ; Z ; D ; F ; M1 ; M2
end define
这里G1是线性移动的代码（通常输出为G1），G2是刀具半径补偿（通常输出为G41或者G42）D是刀具的半径偏置数值，F是进给率。M1，M2是机床代码[在多轴程序里面还要加上G6,S以及H等指令]。
[$#8226] We RECOMEND that the format should be as follows instead of the above :-
define block move linear
N ; linear ; G2 ; x coord ; y coord ; z coord ; tool radius ; feedrate ; M1 ; M2
end define
[$#8226] The radius compensation will need to be added to the majority of options as this is missing in the source files and is specifically required for PowerMill 2D radial leads in/out linear extension compensation setting. ( Many machine tool controls cannot apply a radial compensation on an arc, only on a straight line )
A feedrate is usually required to be output for a linear move.
The first move after a tool change is always treated as a special case. ( This is normally a Rapid Move function but can overlap, especially in multi-axes options. In these cases the Linear Block will need special attention, see tool change )
Linear travel limits may be set and a warning message will appear if the X, Y or Z values exceed these limits. ( The default limits in DUCTpost are usually set at -999999. and 999999. for all axes. See Limits )
A check is made on the change in angle between each move and the next so that it is possible to output a constant contour speed code ( e.g. M90 on the Heidenhain) for moves where the change in angle is small.
[$#8226] NOTE : All multi-axes moves are treated as Linear so it will be necessary to add the angular axes :- azimuth axis ; elevation axis to the above.
我们建议用下面的定义取代上面的线性移动定义方法。
define block move linear
N ; linear ; G2 ; x coord ; y coord ; z coord ; tool radius ; feedrate ; M1 ; M2
end define
在绝大多数情况下半径补偿的指令在原处理程序中都没有定义，但是在左PM两维加工的时候，切入切出必须带半径补偿，如果没有可能会造成过切等结果。（许多机床处理器在圆弧的部位不能够进行半径补偿，而只能在直线的部位进行半径补偿。）F数值通常都跟在线性移动的程序行的后面。
在换刀后的第一次移动通常要特殊对待。（）
线性移动的极限值要定义，如果X Y Z的数值超多极限值系统将要产生报警信息（超行程）。缺省状态下DUCTpost通常把轴的极限数值设为-99999～99999。参考（Limits）
为了输出固定的连续的轮廓程序必须设定一个最小忽略角度，用来检查两个线性移动之间的角度数值是否可以忽略。比如说在Heidenhain里面定义为M90。 |
发表于 2003-11-8 11:49:49
QQ好友和群
QQ空间
腾讯微博
腾讯朋友
收藏
淘帖
赞一下！
发表于 2003-11-8 11:52:03
