iCAx开思网

标题: 【分享】Surfcam Tips 小技巧 [打印本页]

作者: sinderal 时间: 2004-2-20 15:40
标题: 【分享】Surfcam Tips 小技巧
1. 2D Lathe Programming from a Surface Model

Many CAD systems, especially Solids-based systems are being used to design parts that must be machined on a Lathe or MillTurn center.  When imported you are presented with a collection of surfaces and no 2D profile.

There is a quick and easy solution.

The procedure is as follows:

  Import your geometry and re-orient it into a view and location suitable for SURFCAM’s lathe toolpath generators, i.e. World(X) = centerline of rotation = Machine(Z) and World(Y) = cross-slide axis = Machine(X)
Set your Cview to 2 (Front).

Make a new layer and set it as the current layer. (recommended).

  Set your active color different than the model (recommended).

  From the Main Menu, select Create-Spline-CrossSection.

  You’ll be prompted for the “Surfaces To Project Across”, then a dialog box will appear where you can set the Increment between sections – set the increment larger than the maximum radius of your part to avoid unnecessary section creation

  Finally, you’ll be prompted to pick two locations that represent the centerline of your part, after which you’ll see Splines that represent the 2D profile of your part.

作者: sinderal 时间: 2004-2-20 15:45
2. Backup Batch File

Tired of manually backing up your SURFCAM Support Files?  This batch file will automatically backup the Primary SURFCAM Support files.

Since SURFCAM can be installed in many locations we have made this script to run from the SURFCAM folder, no matter where it is installed.

Create a Surfcam-Backup.txt file in your SURFCAM Folder
Open the Surfcam-Backup.txt file
Copy the Script below and paste it into the txt file
Save and close the file
Rename the file to Surfcam-Backup.bat
Double click the Surfcam-Backup.bat file, a DOS window will appear displaying the running script.
A copy of your Primary SURFCAM Support Files will be copied into a C:\SurfcamBakupFiles\ folder.

You may edit this script to have a different destination folder or add additional files to be copied.

**********************************************

; Place this file in your SURFCAM folder

CD Postlib

xcopy "postform.m" "c:\SurfcamBackupFiles\" /Y
xcopy "postform.e" "c:\SurfcamBackupFiles\" /Y
xcopy "postform.l" "c:\SurfcamBackupFiles\" /Y
xcopy "uncx*.*" "c:\SurfcamBackupFiles\" /Y

CD ..

CD Surf2003

xcopy "colors.ini" "c:\SurfcamBackupFiles\" /Y
xcopy "hotkeys.ini" "c:\SurfcamBackupFiles\" /Y
xcopy "surfcam.pst" "c:\SurfcamBackupFiles\" /Y
xcopy "surfcam.ini" "c:\SurfcamBackupFiles\" /Y
xcopy "dgtztlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "drilltlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "edmtlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "lathetlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "ldrlltlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "material.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "milltlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "material.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "plungeroughtlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "threadmilltlb.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "material.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "srmmat.mdb" "c:\SurfcamBackupFiles\" /Y
xcopy "srmtlb.mdb" "c:\SurfcamBackupFiles\" /Y

CD Mpost

xcopy "post.ini" "c:\SurfcamBackupFiles\" /Y

CD ..
CD Spost

xcopy "config.tbl" "c:\SurfcamBackupFiles\" /Y

CD ..
CD SDNC

xcopy "sdnc.sdnccfg" "c:\SurfcamBackupFiles\" /Y

**********************************************

作者: sinderal 时间: 2004-2-20 15:47
3. Restoring SEDIT associations lost after Predator Installation

Open Windows Explorer (or My Computer)

From the Tools menu choose Folder Options

Select the File Types tab

This is a list of all the extensions on your computer. Scroll to the NCC extension (or whichever extension you wish to change) The NCC probably has a small red gear looking icon, this means it opens with predator.

Click on the NCC extension in the list then click the Change button.

This will bring up a list of programs to re-associate the NCC file with. If SEDIT is installed, it is most likely in this list. If you know it's installed but it's not on the list you can click Browse and specify the location of the sedit.exe file.

Click on SEDIT and then click the OK button. NCC files will now open with sedit.

OR…

If you have Windows XP right-click on any ncc file and choose Open With > Choose Program > Select SEDIT and check the box that says "Always use the selected program to open this type of file". NCC files will now open with sedit.

作者: sinderal 时间: 2004-2-20 15:48
4. Adding the CVIEW to the title of an op in the Operation Manager

Open C:\SURFCAM\SURF2002PLUS\NCDefault\Current.ini in an editor like Notepad.
Press F3 to "Find" and search for "commentwithtool"
You will find "commentwithtoolcviewref=0"
Change this to ""commentwithtoolcviewref=3"
SURFCAM will now display the CVIEW each operation was done in.

Other options...

commentwithtoolcviewref=0 No Tool No CVIEW
commentwithtoolcviewref=1 YES Tool NO cview
commentwithtoolcviewref=2 No Tool Yes cview
commentwithtoolcviewref=3 Yes Tool Yes Cview

作者: sinderal 时间: 2004-2-20 15:49
5. Setup Sheets: Using the old text based style in 2002 Plus and 2003
To revert to the old setup sheet style...

Version 2003 only...

In Surfcam go to Tools>Options>Files>Setup Sheets
There you will find a drop down menu for the different styles of setup sheets.

Version 2002 Plus...

Open C:\SURFCAM\SURF2002PLUS\SURFCAM.INI in an editor like Notepad.
Press F3 to "Find" and search for "setup"
You will find "SetupSheet=1"
Change this to "SetupSheet=2"
SURFCAM will now output the old style setup sheet(non html) which can be edited in any standard text editor.

作者: zzhzzhzzh 时间: 2004-4-12 12:46

sinderal wrote:
1. 2D Lathe Programming from a Surface Model
  
  Many CAD systems, especially Solids-based systems are being used to design parts that must be machined on a Lathe or MillTurn center.  When imported you are presented with a collection of surfaces and no 2D profile.
  
  There is a quick and easy solution.
  
  The procedure is as follows:
  
  Import your geometry and re-orient it into a view and location suitable for SURFCAM’s lathe toolpath generators, i.e. World(X) = centerline of rotation = Machine(Z) and World(Y) = cross-slide axis = Machine(X)
  Set your Cview to 2 (Front).
  
  Make a new layer and set it as the current layer. (recommended).
  
  Set your active color different than the model (recommended).
  
  From the Main Menu, select Create-Spline-CrossSection.
  
  You’ll be prompted for the “Surfaces To Project Across”, then a dialog box will appear where you can set the Increment between sections – set the increment larger than the maximum radius of your part to avoid unnecessary section creation
  
  Finally, you’ll be prompted to pick two locations that represent the centerline of your part, after which you’ll see Splines that represent the 2D profile of your part.
   

请问老大，我怎么试验不出来呢？

作者: zzhzzhzzh 时间: 2004-4-12 12:53
1.solidworks图形

作者: zzhzzhzzh 时间: 2004-4-12 12:54
2。输入到SurfCAM中，并变换

作者: zzhzzhzzh 时间: 2004-4-12 12:55
3。cview=2
使用Create > spline >crosssection

作者: zzhzzhzzh 时间: 2004-4-12 12:56
4.

作者: zzhzzhzzh 时间: 2004-4-12 12:56
5.还是要手工连接端点，构成轮廓线。

作者: sinderal 时间: 2004-4-12 22:52
給我SolidWorks的sldprt檔案...我做給你看

作者: zzhzzhzzh 时间: 2004-4-13 11:18
prt & Igs

作者: sinderal 时间: 2004-4-13 12:56
自己按教程試試看 ....

作者: zzhzzhzzh 时间: 2004-4-14 12:19
现在对了，我知道其原理了。第9楼我方向选择错误。

作者: sinderal 时间: 2004-6-8 10:55
Surfcam Multi-Speed

Edit your post processor to allow multiple RPM Speed codes for the same tool.
Example : You have several pockets and counter-bores that you wish to do with the same tool but you would prefer to use several RPM speeds for the different features. In order to achieve this you must modify your post processors with 3 new lines of code.

First open the windows explorer and locate your Postform.m file. Normally it can be found in the C:\SURFCAM\Postlib\ directory. Double click the Postform.m file and it should open in a text editor. Scroll down until you get to the infeed section then type in the three lines shown in bright blue below. This must be done to each post in your postform.m file. ( It is always a good Idea to save a backup of your file before you edit it.)

Infeed
G[Side] X[H] Y[V] D[DComp] F[FRate]
end

Upon [Speed]
S[Speed]
End

Outfeed
G1 G40 X[H] Y[V]
end

作者: sinderal 时间: 2005-5-23 19:13
Posthaste Rotation Angles

Setting up Posthaste for correct Rotation Angle Output:
There is a possibility of incorrect rotary angles being output with "CView Machining" (4 axis indexing of 2 axis toolpaths). The following provides a thorough look at the Posthaste and SURFCAM settings for proper rotational output.



--- Fact # 1 ---

The SET AXIS command in SURFCAM defines a vector that shows which direction the indexer is facing.



Examples:

(0,0,0) (1,0,0) indicates that the indexer is on the left end of the machine table (X-), facing towards the right (X+) end.

(0,0,0) (-1,0,0) (or [1,0,0] [0,0,0]) indicates that the indexer is on the RIGHT end of the machine table (X+), facing towards the LEFT (X-) end.

NOTE: The latter is the "default" setup that most vertical machines use.





--- Fact # 2 ---

The INDEX statement in the post template (PostForm file) indicates which end of the table the indexer is on, which is the OPPOSITE way it is facing.

To set up SURFCAM and the post for the most common  4 axis setup (the latter of the above examples) you would use the following settings:

In SURFCAM , SET AXIS should be (0,0,0) (-1,0,0) or an equivalent value such as (1,0,0) (0,0,0), which is typically facing to the left towards X-, on a standard vertical mill.

In PostForm.m , use  INDEX X  to indicate that the indexer is on the X+ (right) end of the machine table, which means that it is facing left, matching the above “Set Axis” data.



--- Fact # 3 ---

For consistent correct angle output, the SET AXIS data in SURFCAM must be describing the same rotary table orientation as the PostForm file. While SURFCAM’s vector indicates which direction the indexer is facing, the INDEX line in the template tells the post where the indexer is.

Both areas describe the same data in 2 different ways. To make sure these 2 elements match, keep the following in mind when setting the SET AXIS and INDEX values.

If the Set Axis vector is pointing towards X+, Use "Index X-".

If the Set Axis vector is pointing towards X-, Use "Index X".

NOTE: You must apply the same logic to "B axis" (typically horizontal mill) indexing - using INDEX Y or Y- accordingly.

If you need to reverse the sign to a positive or a negative on the rotary angle, use the MULT -1 modifier on the letter A or B. Do NOT just add or take away the “minus” on the INDEXline in the template.

The default SURFCAM installation has the SET AXIS data as follows in the configuration settings (Tools, Options, NC Defaults, 4 axis, Rotary Options) . For a typical "rotary table on the right" setup we would simply compensate for this by setting the post template to Index X-. Again, you can use the Mult -1 modifier if you need to reverse the sign on your rotary axis letter.

作者: sinderal 时间: 2005-5-23 19:16
2005 SolidWorks Associativity

One Button Transfer Utility:
The "One Button" transfer utility is not required for associativity between SolidWorks and SURFCAM 2005. Opening a SolidWorks file directly in SURFCAM will make that file automatically associative. The "One Button" can still be used as an alternate means of associativity. There is a newer "One Button" utility on the SURFCAM web site for all "Sales Partners", under the category "SURFCAM".

作者: sinderal 时间: 2005-5-23 19:26
How To Choose The Proper Lathe Tool:

There are two things to remember when choosing a lathe tool.  The default operation (cutting direction) of the tool and the default orientation (mounting angle) of the tool.  Both of these settings default the tool to the proper angle and cutting direction. These settings can be found by editing the tool.  The description of the tool by its naming convention usually implies the cutting direction and mounting angle, unless it has been previously edited.  Below are examples of the cutting directions and mounting angles.



DEFAULT OPERATION (cutting direction).  Blue indicates approach while green indicates cutting direction

作者: sinderal 时间: 2005-5-23 19:28
DEFAULT ORIENTATION (mounting angle).  Editing the tool and typing in the desired angle can easily change the mounting angle.

NOTE: A negative opposite value can be used. Example: A -45 degrees can be used in place of 315 degrees.

作者: sinderal 时间: 2005-5-23 19:33
2 Axis Milling: Air Wall

How to machine open pockets:
There are situations when one needs to machine steps or "open pockets" on parts. A commonality between these features is that they are not entirely closed. The "missing" walls are commonly referred to as "check" or "air" walls. SURFCAM allows for easy machinery of these part features. A detailed explanation of the entire process and examples will be discussed below.

Steps to machine this feature in SURFCAM:
Using 2-Axis Contour, select the blue inner profile "A" as shown above; note that by default the Select Chain mode is set to "

art"
Change mode to Material and then select the red profile "B", which defines the shape of the air wall
Press Done for chain selections and the 2-Axis Contour dialog box will appear
On the [Tool Info] tab page set the tool, feeds and speeds
On the [Cut Control] tab it is critical that the "Amount to Remove - On Sides" is set to a value that is greater than the distance from the part to the material boundary
Press OK, the resulting tool path is shown in the rightmost picture

作者: sinderal 时间: 2005-6-1 10:10
21樓, 上面功能, 我做的AVI 教程
壓縮檔一

作者: sinderal 时间: 2005-6-1 10:12
21樓, 上面功能, 我做的AVI 教程
壓縮檔二

作者: sinderal 时间: 2005-6-8 08:57
Adjusting Arc Centers in Edit NC

--------------------------------------------------------------------------------

Question:
My file looks correct in SURFCAM but after posting and Back Plotting in Edit NC, large arcs appear in the Back Plotted code.

Answer:
The default for the Back Plot arc center option is set to "Auto". This means that the editor tries to determine arc center location methods automatically i.e. “I,J relative to start point”, “I,J absolute”, etc. This is possible for the vast majority of arcs, unfortunately there is no perfect method for doing this. In cases like this where the user suspects a problem with the Backplot, the arc center type should be set manually. To set this option, select ANALYSIS > BACKPLOT > SETUP > BASIC OPTIONS > select “Relative To Start Point” for the “I,J,K Usage On G2/G3:”.

作者: sinderal 时间: 2005-7-9 14:48
更改4 Axis後處理 MPost的參數 --- MOD命令的應用:

在surfcam四軸後處理 xxxxx.M4裡, 以4軸 A軸為例,
通常位址碼設置如下:

% 00
/ 00
O >4
N >4
G >2
g >2 G
X ->4.>3
Y ->4.>3
Z ->4.>3
z ->4.>3 Z
A ->3.>3
I ->4.>3
J ->4.>3
K ->4.>3
......

當你連續切削往往A軸較度值在後面會出現非常大的值(不管是正值或負值)
例如: X45.34 Y22.343 Z40. A-99998.945 機床就會報警..
可以更改控制器A軸參數讓A軸一直都是 0 -- 359.999 或 0 --- -359.99 然後又是 0 --- 359.999 或 0 --- -359.999,
也就上面那行程序變成
X45.34 Y22.343 Z40. A-278.945

在Surfcam的後處理文件在A軸位址碼那行要加入MOD命令如下:
% 00
/ 00
O >4
N >4
G >2
g >2 G
X ->4.>3
Y ->4.>3
Z ->4.>3
z ->4.>3 Z
A ->3.>3 mod 360
I ->4.>3
J ->4.>3
K ->4.>3

作者: sinderal 时间: 2005-7-9 15:03
原來後處理出來的程序:
%
O1
G17 G40 G80 G90
G91 G28 Z0
N1 T12 M6
( Tool Radius 5. Tool Diam 10. Corner Rad. 5. )
M3 S7958
G0 G90 G54 X-200.089 Y40.621 A-81.655
G43 Z66. H12
M8
G0 Z6.835
G1 Z4.335 F1114.120
Y38.121
X-200.116 Y37.705 Z4.28 A-81.735 F2387.400
X-200.14 Y37.289 Z4.231 A-81.81
X-200.159 Y36.873 Z4.182 A-81.885
X-200.168 Y36.457 Z4.134 A-81.96
Y35.833 Z4.063 A-82.072
X-200.163 Y34.793 Z3.948 A-82.259
X-200.155 Y33.128 Z3.771 A-82.558
X-200.147 Y31.462 Z3.603 A-82.856
X-200.133 Y28.307 Z3.309 A-83.422
X-200.118 Y25.149 Z3.046 A-83.987
X-200.117 Y24.79 Z3.018 A-84.051
X-200.102 Y21.628 Z2.789 A-84.616
X-200.089 Y18.464 Z2.592 A-85.181
X-200.075 Y15.297 Z2.425 A-85.745
X-200.062 Y12.128 Z2.29 A-86.31
X-200.059 Y11.417 Z2.264 A-86.437
X-200.046 Y8.247 Z2.168 A-87.002
X-200.033 Y5.076 Z2.102 A-87.567
X-200.02 Y1.905 Z2.068 A-88.132
X-200.008 Y-1.265 Z2.065 A-88.698
X-200.005 Y-1.977 Z2.068 A-88.824
X-199.993 Y-5.146 Z2.103 A-89.39
X-199.982 Y-8.314 Z2.17 A-89.955
X-199.977 Y-9.51 Z2.203 A-90.169
X-199.975 Y-10.293 Z2.233 A-90.341
X-199.966 Y-10.428 Z2.091 A-89.557
X-199.969 Y-10.47 Z2.143 A-89.844
X-199.98 Y-10.479 Z2.341 A-90.925
X-200.001 Y-10.441 Z2.723 A-93.015
X-200.039 Y-10.321 Z3.383 A-96.656
X-200.059 Y-10.231 Z3.748 A-98.697
X-200.098 Y-10.02 Z4.421 A-102.507
X-200.135 Y-9.767 Z5.056 A-106.184
X-200.177 Y-9.424 Z5.76 A-110.396
X-200.217 Y-9.031 Z6.437 A-114.608
X-200.256 Y-8.591 Z7.084 A-118.823
X-200.291 Y-8.138 Z7.657 A-122.758
X-200.327 Y-7.609 Z8.236 A-126.986
X-200.361 Y-7.038 Z8.775 A-131.225
X-200.393 Y-6.427 Z9.272 A-135.473
X-200.416 Y-5.938 Z9.62 A-138.708
X-200.444 Y-5.27 Z10.031 A-142.936
X-200.47 Y-4.573 Z10.393 A-147.174
X-200.492 Y-3.849 Z10.703 A-151.427
X-200.506 Y-3.33 Z10.888 A-154.397
X-200.524 Y-2.573 Z11.105 A-158.646
X-200.539 Y-1.801 Z11.266 A-162.889
X-200.551 Y-1.02 Z11.369 A-167.13
X-200.558 Y-0.418 Z11.409 A-170.365
X-200.564 Y0.373 Z11.41 A-174.615
X-200.567 Y1.162 Z11.352 A-178.87
X-200.567 Y1.945 Z11.237 A-183.131
X-200.565 Y2.542 Z11.108 A-186.419
X-200.559 Y3.304 Z10.891 A-190.688
X-200.55 Y4.046 Z10.618 A-194.946
X-200.538 Y4.765 Z10.293 A-199.193
X-200.528 Y5.291 Z10.013 A-202.398
X-200.511 Y5.962 Z9.597 A-206.644
X-200.493 Y6.536 Z9.183 A-210.46
X-200.471 Y7.141 Z8.677 A-214.712
X-200.449 Y7.631 Z8.207 A-218.375
X-200.423 Y8.159 Z7.624 A-222.619
X-200.394 Y8.642 Z7.006 A-226.851
X-200.364 Y9.077 Z6.355 A-231.073
X-200.338 Y9.388 Z5.817 A-234.419
X-200.305 Y9.729 Z5.126 A-238.577
X-200.271 Y10.014 Z4.414 A-242.718
X-200.236 Y10.244 Z3.685 A-246.847
X-200.213 Y10.363 Z3.205 A-249.521
X-200.184 Y10.46 Z2.62 A-252.745
X-200.174 Y10.462 Z2.427 A-253.804
X-200.169 Y10.374 Z2.325 A-254.365
X-200.174 Y10.091 Z2.454 A-253.645
X-200.169 Y9.463 Z2.422 A-253.834
X-200.157 Y7.697 Z2.375 A-254.15
X-200.136 Y4.535 Z2.316 A-254.714
X-200.116 Y1.371 Z2.287 A-255.279
X-200.111 Y0.632 Z2.285 A-255.411
X-200.091 Y-2.533 Z2.295 A-255.976
X-200.071 Y-5.698 Z2.336 A-256.541
X-200.067 Y-6.433 Z2.349 A-256.672
X-200.047 Y-9.598 Z2.429 A-257.236
X-200.028 Y-12.765 Z2.539 A-257.801
X-200.009 Y-15.931 Z2.68 A-258.365
X-199.991 Y-19.096 Z2.853 A-258.929
X-199.983 Y-20.552 Z2.942 A-259.188
X-199.965 Y-23.712 Z3.16 A-259.752
X-199.947 Y-26.864 Z3.409 A-260.317
X-199.93 Y-30.008 Z3.69 A-260.883
X-199.913 Y-33.144 Z4.002 A-261.45
X-199.905 Y-34.629 Z4.161 A-261.719
X-199.896 Y-36.387 Z4.337 A-262.003
X-199.888 Y-37.938 Z4.383 A-262.079
X-199.883 Y-38.018 Z5.48 A-263.732
X-199.877 Y-37.869 Z7.056 A-266.111
X-199.868 Y-37.443 Z9.587 A-269.96
X-199.861 Y-36.85 Z12.082 A-273.809
X-199.858 Y-36.508 Z13.261 A-275.65
X-199.852 Y-35.67 Z15.689 A-279.504
X-199.848 Y-34.67 Z18.055 A-283.356
X-199.844 Y-33.122 Z21.04 A-288.399
X-199.843 Y-31.762 Z23.226 A-292.259
X-199.843 Y-30.261 Z25.316 A-296.118
X-199.844 Y-28.623 Z27.299 A-299.976
X-199.846 Y-26.856 Z29.17 A-303.838
X-199.85 Y-24.966 Z30.918 A-307.702
X-199.855 Y-22.965 Z32.532 A-311.56
X-199.858 Y-21.76 Z33.403 A-313.791
X-199.864 Y-19.594 Z34.799 A-317.656
X-199.871 Y-17.343 Z36.044 A-321.516
X-199.881 Y-14.291 Z37.433 A-326.544
X-199.889 Y-11.875 Z38.313 A-330.396
X-199.898 Y-9.398 Z39.029 A-334.254
X-199.906 Y-6.869 Z39.579 A-338.12
X-199.911 Y-5.586 Z39.79 A-340.06
X-199.919 Y-3.19 Z40.067 A-343.673
X-199.929 Y-0.96 Z40.189 A-347.061
X-199.941 Y0.933 Z40.19 A-350.012
X-199.956 Y2.242 Z40.127 A-352.249
X-199.966 Y2.255 Z40.116 A-352.534
X-199.994 Y1.119 Z40.133 A-351.969
X-199.996 Y0.974 Z40.133 A-351.976
X-199.998 Y0.566 Z40.133 A-352.028
X-199.982 Y-1.929 Z40.123 A-351.64
X-199.98 Y-2.09 Z40.127 A-351.729
X-199.979 Y-0.58 Z40.185 A-354.199
X-199.979 Y1.471 Z40.161 A-357.355
X-199.98 Y3.72 Z40.006 A-360.771
X-199.982 Y6.366 Z39.653 A-364.779
X-199.985 Y8.9 Z39.138 A-368.649
X-199.988 Y11.388 Z38.453 A-372.513
X-199.992 Y13.82 Z37.603 A-376.376
X-199.996 Y16.189 Z36.591 A-380.239
....
....

作者: sinderal 时间: 2005-7-9 15:04
更改後處理後所產生的程式:
%
O1
G17 G40 G80 G90
G91 G28 Z0
N1 T12 M6
( Tool Radius 5. Tool Diam 10. Corner Rad. 5. )
M3 S7958
G0 G90 G54 X-200.089 Y40.621 A-81.655
G43 Z66. H12
M8
G0 Z6.835
G1 Z4.335 F1114.120
Y38.121
X-200.116 Y37.705 Z4.28 A-81.735 F2387.400
X-200.14 Y37.289 Z4.231 A-81.81
X-200.159 Y36.873 Z4.182 A-81.885
X-200.168 Y36.457 Z4.134 A-81.96
Y35.833 Z4.063 A-82.072
X-200.163 Y34.793 Z3.948 A-82.259
X-200.155 Y33.128 Z3.771 A-82.558
X-200.147 Y31.462 Z3.603 A-82.856
X-200.133 Y28.307 Z3.309 A-83.422
X-200.118 Y25.149 Z3.046 A-83.987
X-200.117 Y24.79 Z3.018 A-84.051
X-200.102 Y21.628 Z2.789 A-84.616
X-200.089 Y18.464 Z2.592 A-85.181
X-200.075 Y15.297 Z2.425 A-85.745
X-200.062 Y12.128 Z2.29 A-86.31
X-200.059 Y11.417 Z2.264 A-86.437
X-200.046 Y8.247 Z2.168 A-87.002
X-200.033 Y5.076 Z2.102 A-87.567
X-200.02 Y1.905 Z2.068 A-88.132
X-200.008 Y-1.265 Z2.065 A-88.698
X-200.005 Y-1.977 Z2.068 A-88.824
X-199.993 Y-5.146 Z2.103 A-89.39
X-199.982 Y-8.314 Z2.17 A-89.955
X-199.977 Y-9.51 Z2.203 A-90.169
X-199.975 Y-10.293 Z2.233 A-90.341
X-199.966 Y-10.428 Z2.091 A-89.557
X-199.969 Y-10.47 Z2.143 A-89.844
X-199.98 Y-10.479 Z2.341 A-90.925
X-200.001 Y-10.441 Z2.723 A-93.015
X-200.039 Y-10.321 Z3.383 A-96.656
X-200.059 Y-10.231 Z3.748 A-98.697
X-200.098 Y-10.02 Z4.421 A-102.507
X-200.135 Y-9.767 Z5.056 A-106.184
X-200.177 Y-9.424 Z5.76 A-110.396
X-200.217 Y-9.031 Z6.437 A-114.608
X-200.256 Y-8.591 Z7.084 A-118.823
X-200.291 Y-8.138 Z7.657 A-122.758
X-200.327 Y-7.609 Z8.236 A-126.986
X-200.361 Y-7.038 Z8.775 A-131.225
X-200.393 Y-6.427 Z9.272 A-135.473
X-200.416 Y-5.938 Z9.62 A-138.708
X-200.444 Y-5.27 Z10.031 A-142.936
X-200.47 Y-4.573 Z10.393 A-147.174
X-200.492 Y-3.849 Z10.703 A-151.427
X-200.506 Y-3.33 Z10.888 A-154.397
X-200.524 Y-2.573 Z11.105 A-158.646
X-200.539 Y-1.801 Z11.266 A-162.889
X-200.551 Y-1.02 Z11.369 A-167.13
X-200.558 Y-0.418 Z11.409 A-170.365
X-200.564 Y0.373 Z11.41 A-174.615
X-200.567 Y1.162 Z11.352 A-178.87
X-200.567 Y1.945 Z11.237 A-183.131
X-200.565 Y2.542 Z11.108 A-186.419
X-200.559 Y3.304 Z10.891 A-190.688
X-200.55 Y4.046 Z10.618 A-194.946
X-200.538 Y4.765 Z10.293 A-199.193
X-200.528 Y5.291 Z10.013 A-202.398
X-200.511 Y5.962 Z9.597 A-206.644
X-200.493 Y6.536 Z9.183 A-210.46
X-200.471 Y7.141 Z8.677 A-214.712
X-200.449 Y7.631 Z8.207 A-218.375
X-200.423 Y8.159 Z7.624 A-222.619
X-200.394 Y8.642 Z7.006 A-226.851
X-200.364 Y9.077 Z6.355 A-231.073
X-200.338 Y9.388 Z5.817 A-234.419
X-200.305 Y9.729 Z5.126 A-238.577
X-200.271 Y10.014 Z4.414 A-242.718
X-200.236 Y10.244 Z3.685 A-246.847
X-200.213 Y10.363 Z3.205 A-249.521
X-200.184 Y10.46 Z2.62 A-252.745
X-200.174 Y10.462 Z2.427 A-253.804
X-200.169 Y10.374 Z2.325 A-254.365
X-200.174 Y10.091 Z2.454 A-253.645
X-200.169 Y9.463 Z2.422 A-253.834
X-200.157 Y7.697 Z2.375 A-254.15
X-200.136 Y4.535 Z2.316 A-254.714
X-200.116 Y1.371 Z2.287 A-255.279
X-200.111 Y0.632 Z2.285 A-255.411
X-200.091 Y-2.533 Z2.295 A-255.976
X-200.071 Y-5.698 Z2.336 A-256.541
X-200.067 Y-6.433 Z2.349 A-256.672
X-200.047 Y-9.598 Z2.429 A-257.236
X-200.028 Y-12.765 Z2.539 A-257.801
X-200.009 Y-15.931 Z2.68 A-258.365
X-199.991 Y-19.096 Z2.853 A-258.929
X-199.983 Y-20.552 Z2.942 A-259.188
X-199.965 Y-23.712 Z3.16 A-259.752
X-199.947 Y-26.864 Z3.409 A-260.317
X-199.93 Y-30.008 Z3.69 A-260.883
X-199.913 Y-33.144 Z4.002 A-261.45
X-199.905 Y-34.629 Z4.161 A-261.719
X-199.896 Y-36.387 Z4.337 A-262.003
X-199.888 Y-37.938 Z4.383 A-262.079
X-199.883 Y-38.018 Z5.48 A-263.732
X-199.877 Y-37.869 Z7.056 A-266.111
X-199.868 Y-37.443 Z9.587 A-269.96
X-199.861 Y-36.85 Z12.082 A-273.809
X-199.858 Y-36.508 Z13.261 A-275.65
X-199.852 Y-35.67 Z15.689 A-279.504
X-199.848 Y-34.67 Z18.055 A-283.356
X-199.844 Y-33.122 Z21.04 A-288.399
X-199.843 Y-31.762 Z23.226 A-292.259
X-199.843 Y-30.261 Z25.316 A-296.118
X-199.844 Y-28.623 Z27.299 A-299.976
X-199.846 Y-26.856 Z29.17 A-303.838
X-199.85 Y-24.966 Z30.918 A-307.702
X-199.855 Y-22.965 Z32.532 A-311.56
X-199.858 Y-21.76 Z33.403 A-313.791
X-199.864 Y-19.594 Z34.799 A-317.656
X-199.871 Y-17.343 Z36.044 A-321.516
X-199.881 Y-14.291 Z37.433 A-326.544
X-199.889 Y-11.875 Z38.313 A-330.396
X-199.898 Y-9.398 Z39.029 A-334.254
X-199.906 Y-6.869 Z39.579 A-338.12
X-199.911 Y-5.586 Z39.79 A-340.06
X-199.919 Y-3.19 Z40.067 A-343.673
X-199.929 Y-0.96 Z40.189 A-347.061
X-199.941 Y0.933 Z40.19 A-350.012
X-199.956 Y2.242 Z40.127 A-352.249
X-199.966 Y2.255 Z40.116 A-352.534
X-199.994 Y1.119 Z40.133 A-351.969
X-199.996 Y0.974 Z40.133 A-351.976
X-199.998 Y0.566 Z40.133 A-352.028
X-199.982 Y-1.929 Z40.123 A-351.64
X-199.98 Y-2.09 Z40.127 A-351.729
X-199.979 Y-0.58 Z40.185 A-354.199
X-199.979 Y1.471 Z40.161 A-357.355
X-199.98 Y3.72 Z40.006 A-0.771
X-199.982 Y6.366 Z39.653 A-4.779
X-199.985 Y8.9 Z39.138 A-8.649
X-199.988 Y11.388 Z38.453 A-12.513
X-199.992 Y13.82 Z37.603 A-16.376
X-199.996 Y16.189 Z36.591 A-20.239
....
....

作者: sinderal 时间: 2005-7-14 09:22
英制程序變成公制程序:

有些加工程序是由美國或加拿大的英制國家的客戶所提供, 但是操機者希望用公制的程序, Surfcam自帶的NC編輯器可以在裡面將英制程序變成公制程序

欢迎光临 iCAx开思网 (https://www.icax.org/)