资源共享，智能制造。致力于打造一个数控编程行业爱好者的交流平台，积极推广数控编程技术，让每一位数控爱好者学会编程，期待您的加入。
当你点开这篇文章的时候，我们已经上路了........
What are you waiting for ?
——CNC数控编程智造——
一个数控达人聚焦的平台
1MasterCAM 3D 刀路优化
先来看个图片。这个功能是Mastercam于2009年版推出的。正如上面写的一样，这是一个非常重要的功能，但是若干年过去了，这方面的使用还不是很广泛。大多用户还不知道这应该怎么用。今天写一写我对此功能的认知，分享给大家，与君共勉.
这个功能非常适用于在表面光洁度及形位公差要求高的行业，如果合理使用了“高级刀具路径优化”，不仅可以提高工件的表面光洁度，而且还可以显著提升加工效率。高级刀具路径优化功能在每个3D刀路的过滤公差处打开，与X4之前的版本会有不同，但主要的区别还是新增的“平滑性过滤设置”。也是我们需要共同学习的地方。
2原理
我们先来看一组对比刀路，第一个是没有开启，第二个是开启平滑性过滤设置的刀路。
没有开启“平滑性过滤”的刀路，白色点是XYZ位置点，也就是最终G代码中的XYZ坐标点。 绿色线段为线性查补，红色蓝色线段为圆弧插补。
这是开启了“平滑性过滤”的刀路，从上面两个图对比可以明显看出使用了“平滑性过滤”后XYZ位置点明显增多并且更加均布。
正是因为有了更加均匀分布的点，才可以实现匀速加工，加工进给率按照我们设定的F值在一个很小的范围内波动，实现了更高的表面质量和更高的加工效率。没有开启“平滑性过滤”，加工过程中会出现进给率忽快忽慢，从而造成机床的频繁加减速，得到的是较差的加工表面和加工速度的较大损失。合理使用“平滑性过滤”，可以缩短加工时间，提高表面质量。最高可以节省近40%的时间。
3参数
平滑性过滤一共有四个选项。
1.使用固定线段长度。控制刀路关键点，按照指定的线段长度重新分布，使刀路平滑，提高加工效率，减少加工时间。
2.沿着刀具路径任一点偏移。Mastercam会在指定的公差范围内，沿着刀具路径将关键点随机向前向后移动，消除加工表面的波浪效应。
3.点的数量减到最小。顾名思义，将关键点的数量减少到最小。
4.当前圆弧作为线段。将所有路径输出为线性移动插补，适用于没有圆弧插补的机床系统。
4公差
我们设置的整体公差（100%）=切削公差(90%)+圆弧过滤公差(5%)+平滑过滤公差(5%)。占用比例是可以随意调整的，建议使用默认比例。
应用范围：
1.使用固定线段长度：特别适用于高速加工，特别试用于高表面质量要求的工件，不适用于预读取能力差的控制器。
2.沿着刀具路径任一点偏移：适用于消除曲面表面的波浪纹。
3.点的数量减到最小：适用于精度要求一般的情况，比如开粗，残料，半精加工等。适用于预读取能力差的控制器。
4.当前圆弧作为线段：适用于没有圆弧插补指令的数控系统，有圆弧插补指令的数控系统，但在拐角落区域使用圆弧移动反而“跑不快”的机床。
线段长度：
不合理的设置线段长度会造成加工时间延长，加工时机床抖动。
检查方法，降低进给倍率，机床如果不抖动，说明参数设置正常，如果抖动说明设置不合理。
线段长度必须通过计算得出的值要大于机床响应时间，至于机床响应时间，你可以查看机床说明书，或者咨询机床厂商。
计算公式 60*线段长度/F（m/min）=刀路关键点移动时间>机床最小响应时间。
高效加工：永恒的追求
5RCTF径向减薄技术
想必动态铣削带来的震撼,经常关注我博客的各位都深刻感受.那为什么说RCTF 径向减薄技术为Dynamic动态加工注入新动力?
因为有了这项技术,不仅可以让你动态加工效率进步提升,而且还可进一步延长刀具使用寿命.
那么这么奇特技术在那呢?
什么,只有这面一个简单按钮?点开后 转速进给变成灰色不可选?那他到底有是怎么原理呢?
径向减薄
径向减薄技术并非新技术.他是一个真实存在的现象.
在实际编程之中,我们使用的每齿进给量以及线速度,都会按照刀具说明手册的推荐值来提供.
刀具制造商推荐的每齿进给数值是通过进给量精确计算出来的.
在我们编程之时.切宽=刀具直径50%,每齿进给量=实际最大切削厚度.
但只有切削宽度达到或超越刀具直径50%时,实际最大切削厚度才能符合刀具厂商的推荐值.
而我们在编程时,当切宽小于50%时.情况则不然.
当切削宽度为刀具直径10%时,刀具实际最大切削厚度=0.05mm.这时的值,并非是刀具厂商所推荐的.
mastercam的RCTF技术,可以将速度自动提升,当在较薄区域切削时,刀具实际最大切削厚度依旧按照刀具厂商推荐值在运行.这样,有效的提升了整个加工刀路的效率.而且因为有了刀具厂商的最优值为参考,刀具使用寿命也得到了进一步的延长.
6适用范围
在传统的加工之中,开粗时,切削宽度达到刀具直径70%左右是很常见的情况,所以这种情况时,径向减薄技术无用武之地.
而在高速加工中,虽然看起来好像可行,但高速加工的切削状态是不均匀的.在拐角等切削负载波动的地方,容易出现问题.所以径向减薄也并不适用高速区域开粗.
径向减薄最佳适用的是切削宽度屈居于恒定的时候,刀路切削宽度较小,且波动较少时,径向减薄技术,可以让生产效率的到一个飞跃.而动态加工正好满足这样的需求.
7精要总结
有了径向减薄技术的动态加工,我们不需要在盲目的设定切削参数,合理的切削参数可以让刀具使用寿命更长.而更加薄的切宽,通过径向减薄技术反而可以带来更加高的效率.
这几天正好对这功能做了一些试切,效果很是令我满意.具体细节,等以后整理出来,在跟大家分享.
MasterCAM动态 :新工艺溶于新软件中
8平行加工刀路的前生与今世
平行精加工可以说是很常见的一种加工策略.本篇文章的目的是让大家了解和熟悉在传统和高速精加工中,平行精加工的区别.
图档如下:
简单的一个图形,我们使用平行精加工策略.
使用直径6的球刀,间距3mm,公差0.01,获得刀路如下:
好象没有什么不妥~~
就实际加工而言,首先在工件表面垂直进刀,是不允许的,我们可以修改下进退刀选项.
我们打开曲面参数,设定进退刀信息如下:
重新计算刀路.
想点样子咧~但是两层连接部分的连接还是不符合我们的需求.在工件上连接会产生刀纹,这个图形外围没干涉,所以不会产生惯性过切.我们需要对连接进一步调整.
我们打开连接设置,在默认参数下设置连接切线为3mm.计算刀路。
计算得到刀路如下:
连接是出来了,但这种垂直的连接方式,还是会造成机床运动时减速,浪费加工时间,我们需要圆弧方式进行连接.
于是继续修改!将连接方式从默认打断改为平滑.去掉切线长度.
计算刀路得到刀路如下:
现在 得到的切入切出,层刀路之间的连接过度都是我们需要的了.但拐角之间的刀路是无法进行修剪的.
如图所示,这里存在大量的刀路突然转向.这是我们不希望看到的.
好了 传统的精加工平行加工设置就到这里结束了.我们再来看看高速精加工平行设置.
选用3D高速刀路-平行.
选择直径6的球刀,设置切削间距为3mm,设定公差0.01 其他默认,计算刀路.
高速中漂亮的垂直圆弧切入切出,层连接圆弧连接,完全不需要我们操心.下面我们就再次动手,把拐角修掉.
展开圆弧过滤/公差,选择刀路修圆.启用刀路修圆.
使用依照半径,设置半径为4.0
计算刀路.
看拐角都有增加R1的圆角.(额,为什么是R1而不是设定的R4呢?因为其中R3是抵消刀具的R3~)。
9精要总结
由此可见,高速加工刀路,不但在计算方面有优势(支持后台计算,是传统刀路不支持的),设置简单,而且刀路更加合理.
当然,高速的优势还不止这些.还需要大家深入挖潜!
102D、3D进给自适应功能
Mastercam Machine Dynamic and HighFeed 为2D、3D进给自适应功能（包括拐角进给加减），HighFeed优化原理根据恒金属去除率调整进给，在拐角处缓减、缓加进给，进而平滑拐角进给，在空切时加快进给，提高效率，总之使用后加工时间稍微增长，加工质量可得到改善。
用Highfeed前，先设置好Mastercam Machine Dynamic参数 ，各参数释意如下。如只是优化精加工，无需设置STL，直接点击Highfeed图标，再点击运行图标即可。
Feedrate smoothing 进给平滑
Recombine segments when feed rate changes less than 当加减速进给变化率小于设定值时，合并成一个单节，一般为10%。
If the feed rate of a segment changes less than this percentage, compared to the previous segment in the toolpath, the segments are combined into a single line or arc. The suggested setting is 10%.
Look-ahead (% of tool diameter) 单节段长值（刀具直径的百分比）
Breaks the toolpath into segments whose maximum length is the look-ahead distance. This parameter slows the feed rate before reaching an area where the tool is buried. Larger values increase the distance for slowing down into and accelerating out of corners. The suggested setting is 10%.
单节段长值，拐角处打成若干段，越到转角点越慢。单节段长值越大，加减速距离越长，推荐10%刀具直径百分比。
Max feed rate change per block in/min mm/min 单节进给变化量
Limits the feed rate changes in each block. Smaller values increase the number of segments, thereby increasing the distance for slowing down into and accelerating out of corners. The suggested setting is 20.
限定单节进给变化量，值越小，节点越多，加减速距离越长，推荐荐500mm/min 20in/min。
Accelerate to smooth feed rates 启用机床加减速再细分
Allows the machine to slow down gradually as it approaches a corner and speed up gradually after leaving a corner. It breaks the toolpath into smaller segments than it has already been broken into by the look-ahead value. The maximum feed rate change per block is limited by the acceleration value.
用机床加减速处理拐角进给，进一步细分。单节速度变化由机床加减速值决定。
Note: This option is not advised for controls that have a slow processing speed. For these controls, this option could result in a longer processing time since it produces more blocks to process.
说明：此操作算法计算时间稍微变长，软件不作警告。
Segment length % of tool diameter 细分单节段长（刀具直径百分比）
Segments longer than this value are broken into shorter segments. This parameter is only available if you choose the Accelerate to smooth feed rates option.
拐角处单节段长超过设定值时，用设定值进一步细分，仅当启用机床减速细分进给时有效。
11Cornering拐角参数
Slow to min. cornering feed rate when direction changes 当转角角度大于设定角度时，拐角点进给降到最小
When the toolpath approaches an area where the direction changes more than this value, the feed rate is reduced to the minimum cornering feed rate.
Minimum cornering feed rate 最小进给值
Sets the feed rate to use at sharp corners and small-radius arcs.应用于尖角和小圆弧
Cornering acceleration 机床加减速值
Opens a dialog box where you can enter the maximum feed rate for corners and arcs before causing axis over-travel.
12Highfeed 应用
NC代码
%
T (T)
(PROGRAMMER TA )
(2012-11-02 16.02)
(T219 - H219 - D10. - END MILL )
N10 ( 2D-CONTOUR )
G0 G40 G49 G80 G90
T219 M06(EM DR-10R0)
/M08
(MAX=Z25.)
(MIN=Z0.)
(STOCK XY= 0. Z = 0.)
G0 G90 G54 X-107.743 Y-8.633 S3500 M03
G43 H219 Z25.
Z2.
G1 Z0. F500.
X-108.41 F300.
X-109.077 F800.
X-109.743
G2 X-111.743 Y-6.633 R2. F300.
G1 Y-5.637 F800.
Y-4.64 F1000.
Y28.252
Y29.249 F800.
Y30.245 F300.
X-110.745
X-109.747 F800.
X-108.749 F1000.
X5.023
X28.632 Y16.614
X29.475 Y16.128 F800.
X30.319 Y15.641 F300.
G3 X29.556 Y15.014 R33.404
X28.812 Y14.364 R33.404 F800.
X18.205 Y-16.017 R33.403
X18.383 Y-16.988 R33.404 F300.
G1 X17.388
X16.393 F800.
X15.398 F1000.
X-39.323
X-40.318 F800.
X-41.313 F300.
G2 X-41.879 Y-16.173 R15.008
X-42.39 Y-15.323 R15.008 F666.8
X-42.562 Y-1.041 R15.008
G1 X-40.563 Y2.762 F1000.
X-40.163 Y3.522 F800.
X-39.764 Y4.283 F300.
X-40.584 Y4.537
X-41.405 Y4.791 F800.
X-42.226 Y5.045 F1000.
X-45.509 Y6.062
G3 X-76.468 Y-18.451 R23.938 F791.1
X-76.38 Y-19.435 R23.937 F300.
G1 X-77.243 Y-19.933
X-78.105 Y-20.431 F800.
X-78.968 Y-20.929 F1000.
X-110.018 Y-38.856
X-110.881 Y-39.354 F800.
X-111.743 Y-39.852 F300.
Y-38.875
Y-37.898 F800.
Y-36.921 F1000.
Y-7.61
Y-6.633 F800.
G2 X-109.743 Y-4.633 R2. F300.
G1 X-108.41 F800.
X-107.743 F300.
G0 Z25.
M05
M09
G91 G28 Z0.
G28 Y0.
M30
%
11圆弧过滤及过滤公差
Arc Filter/Tolerance page圆弧过滤及过滤公差
Use this page to control toolpath tolerances. Typically, this involves several sets of variables. Not all parameters listed are available for every toolpath type.
选项用于设置过滤公差，通常，列出相关的所有项不是所有刀路都需要全部设置。
Note:说明
To learn more about the other options on this page, click the 'Field definitions' tab above.
选择“字段定义”，了解更多的功能。
If 3D Advanced Toolpath Refinement is enabled, use the Refine Toolpath button to access additional options for filtering and smoothing toolpath motion.
如3D刀路优化选项启用，使用该选项过滤和圆滑3D刀路。
Filter ratio and total tolerance过滤比例和整体误差
Mastercam is a total tolerance system, based on the sum of the cut tolerance and filter tolerance and the ratio between them. For example, you can tell Mastercam to maintain a 2:1 ratio between the filter and cut tolerance, and a total tolerance of .003 inches. Mastercam automatically sets the filter tolerance to .002 inches, and the cut tolerance to .001 inches. Whenever you change one value, Mastercam automatically updates the others.
整体误差，是切削公差和过滤公差之和。举例，如过滤公差和切削公差比例是2：1，且整体误差是0.003英寸，则过滤公差自动设置为0.002英寸，切削公差自动设置为0.001英寸，当改变其中一项值时，其余选项将自动改变。
Typically, the ratio of filter tolerance to cut tolerance is 2:1. Using the total tolerance prevents assigning too large or too small a ratio of filter tolerance to cut tolerance.
通常，过滤公差和切削公差比例为2：1，应用整体误避免两者之间太大或太小的比例设置。
Select Custom to override the preset ratios with your own specific values for cut and filter tolerance.
选择用户自定义比例，指定切削和过滤公差值。
Select Off to disable toolpath filtering.
OFF关闭过滤
12过滤设置
Toolpath filtering lets you replace multiple very small linear moves — within the filter tolerance — with single arc moves to simplify the toolpath.
过滤功能在于在设定过滤公差范围内去除重复的细微线性差补——以单一的线性或圆弧插补简化刀路。
Use the different checkboxes to enable or restrict arc creation in specific planes.
指定平面启用或禁用圆弧插补
Enter minimum and maximum arc radius values to control the size of the arcs Mastercam creates in the filtered toolpath.
最大最小圆弧用于设置过滤最大和最小过滤圆弧
Toolpath fillets路径拐角圆角
Select the Toolpath fillet option to have Mastercam insert an arc of the specified radius in the toolpath at sharp corners. The radius value that you enter here should be at least as large as the radius of the finish tool. The fillets are created as tool motions only. They are not saved as part of your surface model, and they have no effect on your part geometry.
路径圆角选项在拐角处插入圆角，半径值需设置不小于精加工后的几何体拐角R值。圆角功能仅产生拐角刀路，不改变驱动几何体，对几何体无影响，拐角处路径不能保存为几何体。
13程序过滤及路径圆角
Filtering toolpaths程式过滤
Filleting toolpaths 路径圆角
Use toolpath fillets to create a toolpath which automatically leaves fillets at the corners between the surfaces. The fillets let you maintain smoother tool motion in corners and as the tool transitions between part features. The fillets are created entirely by the programmed tool motion, and have no effect at all on your surface model or part geometry. For many parts, this can be much easier and faster than actually creating the surface fillets in your part geometry. This feature is available for all high speed surface toolpaths. The following picture shows a part with a series of raster cutting passes. You can see the sharp transitions between surface boundaries. Hold your mouse over the picture to see the same toolpath with toolpath fillets applied.
路径圆角功能为自动在曲面拐角处插入圆角，其作用保持刀具在拐角处圆滑过渡，并作用于全部过程，且对驱动几何体无任何影响。对绝大多数工件，无需修改几何体R角，相比修改几何体操作更简单、快捷，此功能所有HST刀路都适用。下图为放射状刀路，未圆角时在拐角处路径为尖角，移动鼠标刀图片显示为圆角后的路径。
Note that the fillets are created not only along the direction of the tool motion, but across it as well. For example, consider a toolpath which machined the inside corner shown here with a series of waterline passes down the walls:
说明：路径拐角圆角不仅引导方向能插入圆角，且截断方向也可以。例如下图，此处加工路径考虑为水线等高策略，
With toolpath filleting turned off, the cutting passes would look like this:
不开启路径圆角功能，刀路如下
运用拐角圆角后，拐角边界处，路径分别在引导和截断方向插入圆角，刀路如下
Toolpath filleting can seem similar to toolpath corner rounding, but there is an important difference. Toolpath filleting looks at your part model to calculate the fillets, while toolpath corner rounding looks directly at the calculated tool motion. For example, if you cut a 6mm fillet with a 12mm ball mill, the toolpath will still have a sharp corner. Toolpath corner rounding, on the other hand, would identify and apply an arc to that corner. To create the fillets, select the Toolpath fillet option on the Arc Filter/Tolerance page and enter the desired radius of the fillets. The radius that you enter here should be larger than the radius of the tool.
路径圆角功能类似于走圆角功能（Corner rounding），但也有一些重要的区别。路径圆角仅在几何体拐角处插入圆角路径，而走圆角算法直接在路径拐角处插入圆角。举例，上图用D12R6球刀刀具加工，在拐角处仍走直角，这种情况下可以用corner rounding直接插入圆角。应用路径圆角功能，选择路径圆角选项并设置合适的R角，R角值要比刀具R角略大些。
14过滤比例及公差
Filter ratio过滤比例
The ratio of filter tolerance to cut tolerance. This ratio is automatically applied to the filter tolerance and cut tolerance. If Off, then Mastercam uses only the cut tolerance for the toolpath.
指过滤公差与切削公差的比例，自动设置两者值，如OFF，刀路仅应用切削公差计算。
Linearization tolerance线性公差
Used when converting 3D arcs and 2D or 3D splines in the chained geometry from curves to lines. Smaller linearization tolerance values make more accurate toolpaths, but may take longer to generate and create a longer NC program. Click here to learn more about setting machining tolerances.
转换串联中3D圆弧、2D或3D曲线成直线段，较小的线性公差，生成更精确的刀路，但增加程序长度和计算时间，点击此处连接，了解更多加工公差设置。
Filter tolerance过滤公差
When a distance between a point in the toolpath and the new line or arc is less than or equal to the tolerance, Mastercam automatically eliminates the tool move from the toolpath. Mastercam continuously eliminates moves until the entire toolpath lies within the maximum tolerance.
源路径中任意一点到过滤后路径中一直线或圆弧的距离小于等于切削过滤公差，MC便自动过滤掉，并在设定的公差范围内连续过滤下去，只至程序结束。
Cut tolerance切削公差
Determines the accuracy of the surface toolpath using chordal deviation to linearize the toolpath. A smaller cut tolerance value creates a more accurate toolpath that may take longer to generate and could result in a longer NC program.
切削公差定义为用控制弦高方式分割曲面线性插补的精度，越小的公差值刀路越精确，但会增加计算时间和程序长度。
15公差设置
Total tolerance (3D)整体公差
Displays the sum of the filter tolerance and cut tolerance.过滤和切削公差之和
The dialog box that opens when you choose the Total Tolerance button depends on whether the 3D Advanced Toolpath Refinement feature is enabled for your Mastercam configuration.
整体公差及过滤选项设置，要根据3D刀路优化功能(Refine toolpath)是否启用，对话框显示不同：
If 3D Advanced Toolpath Refinement is enabled, the Refine Toolpath dialog box displays. Use its options to set additional parameters for filtering and smoothing toolpath motion within the specified total toolpath tolerance.
如启用，显示“Refine Toolpath”按钮，依据整体公差，设置相关过滤和圆滑刀路选项。
If 3D Advanced Toolpath Refinement is disabled, the Total Tolerance dialog box displays. Use its options to adjust the ratio of the filter tolerance to the cut tolerance, change the tolerances, and select arc options.
如未启用，显示为“Total Tolerance”，选择比例选项调整过滤公差与切削公差比例，并设置过滤最大最小圆弧。
Note: Run the Mastercam applet to enable the 3D Advanced Toolpath Refinement feature, or contact your local Mastercam Reseller for assistance.
说明： 启动Mastercam软件控制面板应用程序（Mastercam applet），启动3D刀路优化（Toolpath Refinment）
操作为： 开始->所以程序-〉Mastecam->MCAMX Control panel applet
Total tolerance (2D)整体公差(2D)
Displays the sum of the filter tolerance and cut tolerance.切削和过滤公差之和
If Filter ratio is set to Off, Total tolerance shows only the cut tolerance.
如过滤比例OFF，整体公差为切削公差。
16单向过滤
One way filtering单向过滤
Filters a toolpath in one direction to avoid small polygonal patterns on the finish that can happen with zigzag filtering.
选择单向过滤，防止往复过滤时刀路出现不规整的细微曲折刀路。
Create arcs in XY（在G17平面生成圆弧）
Create arcs in the XY plane. Choose this option if appropriate for your post processor configuration to handle arcs (usually designated as G17 in the NC code).
在XY平面生成圆弧，可生成圆弧的地方过滤后，生成圆弧插补格式NCI，通常后处理生成代码格式为G17 G02/G03 。
Create arcs in XZ（在G18平面生成圆弧）
Create arcs in the XZ plane. Choose this option if appropriate for your post processor configuration to handle arcs (usually designated as G18 in the NC code).
在XZ平面生成圆弧，可生成圆弧的地方过滤后，生成圆弧插补格式NCI，通常后处理生成代码格式为G18 G02/G03 。
Create arcs in YZ（在G19平面生成圆弧）
Create arcs in the YZ plane. Choose this option if appropriate for your post processor configuration to handle arcs (usually designated as G19 in the NC code).
在YZ平面生成圆弧，可生成圆弧的地方过滤后，生成圆弧插补格式NCI，通常后处理生成代码格式为G19 G02/G03 。
Minimum arc radius最小过滤圆弧半径
Determines the minimum radius of any arc added to the toolpath by the arc filter. If an arc is smaller than the minimum arc radius, Mastercam adds lines to the toolpath in place of the arc.
最小圆弧半径定义为，最小过滤圆弧半径，过滤时路径圆弧小于最小圆弧半径时生成线性差补。
Maximum arc radius最大过滤圆弧半径
Determines the maximum radius of any arc added to the toolpath by the filter. If an arc exceeds the maximum arc radius, Mastercam adds lines to the toolpath in place of the arc.
最大圆弧半径定义为，最大过滤圆弧半径，过滤时路径圆弧大于最大圆弧半径时生成线性差补。
Toolpath fillet(unavailable for 2D high speed toolpaths)路径圆角（2D HST不适用）
Select this option to have the toolpath leave fillets between the surfaces in your part. The fillets are created by the toolpath only and do not affect your part model or geometry. Click here to learn more about toolpath fillets and see a diagram.
设置此项，路径在拐角处插入圆角修整，仅修改刀路，对几何体无影响。更详细图文说明，点击连接了解。
Radius(unavailable for 2D high speed toolpaths)半径（2D HST不适用）
Enter the radius of the fillets to be created. Typically, this value should be larger than the radius of the tool.
路径圆角半径，通常，比刀具半径略大。
CNC数控编程 :想说爱你不容易
联系客服
