MillWrite is capable of reading a "command file", which is a list of instructions on what to do. This enables you to use MillWrite on in an automatic or semi-automatic mode.

If you download and install MillWrite, (or this version partially translated into German),
you can download and run this sample command file:
MillWrite-command-file,-cut-triangles-and-engrave.m8c

For two examples of how you can use this feature:

If you have software in your shop that is creating part numbers, and if you need to engrave those part numbers, then that software could create a MillWrite command file that specifies the part number. The software would then call MillWrite with that command file. MillWrite would follow the instructions in that command file, and create a CNC program to engrave that particular part number. This enables you to create CNC programs without any human intervention.

If you find that you are repeatedly doing the same operations over and over, with only a few changes between them, you could create a software program that asks you for the information on how to make the particular part, or what to engrave on the part, and after you have specified those parameters, your software creates a command file for MillWrite.

Your software could then call MillWrite to run that command file, and MillWrite could either leave the job on the screen for you to verify and/or modify, or it could create a CNC program for you.

For example, if you are repeatedly drilling some holes in parts that you are making, but occasionally you have to modify the quantity and/or placement of the holes, you would create a software program that lets you specify the quantity and/or locations for the holes, and after you have specified the information, your software would create a command file for MillWrite that specifies those particular holes to be drilled. This would be easier and more foolproof than create a drilling program yourself for every part.

There are several ways to run command files. Normally you would want to call MillWrite from another software program. This method allows MillWrite to be used automatically by other software.

If you are creating your own software, you can call MillWrite from that software with the name of the command file. For example, in the C language, you would call it like this:

char MillWrite_8_folder[] =  "C:\\MillWrite_8\\";   // folder that has MillWrite_8.exe
char MillWriteCommandFilename[200];

strcpy (MillWriteCommandFilename, "engrave text command file.m8c");
  
ShellExecute( NULL,
                "open",       // Operation to perform
                "MillWrite_8.exe",
                MillWriteCommandFilename,
                MillWrite_8_folder,   
                SW_SHOW);

However, when you are designing and testing your command files, these two methods are the most useful:

• Drag and drop a command file on top of the MillWrite icon.

• At the Drawing page, set one of the User-Defined Buttons to run a command file. Then, when you click that button, it will ask you to select the command file, and when you do, it will run it for you.
If you want the help file for the User Buttons, download all of the help files from this page.

1) Create a CNC file that is saved on the hard disk. MillWrite exits when finished.
2) Create a CNC file that is transmitted via serial port to the CNC controller. MillWrite exits when finished.
3) Create a job file that remains on the computer screen for you to deal with. MillWrite remains  active so that you can see the job file and decide what you want to do with it.

A command file can modify a job that you have previously created and tested. This is useful when you want to do the same job over and over, but each time you want to make some slight change to it. For example, you might want to engrave a particular part over and over, but each time you need to change one or move of the text items, but you do not want to change any of the text locations, tool feed rates, or anything else. In that case, you would use the "open job=" command to open that particular job, and then modify only the items that you want to change.

This is the easiest and most foolproof way of using a command file because you can test the job ahead of time to make sure that you have set everything correctly in regards to the tool's feed rate, the text height, the tools' cutting depth, etc..

Your CNC program will be perfect when you make subtle changes to a job that you have already proven to work correctly.

A command file can create polylines, text to engrave, data matrix barcodes, and other items, so you could create whatever you need. MillWrite will give each new item whatever defaults you have set in MillWrite, and you can override any of those defaults with the command file, if you need to.

If your default feed rate, tool number, text type, and other parameters have been set appropriately, then this is an easy way to create programs to engrave some tax, or to cut a logo.

• The command file is a plain text file that lists the commands one after the other.

• The commands are processed in the order that they are listed, just like a human follows a list of instructions.

• The commands can use upper and/or lower case.

• There are two types of commands:

1) Commands that have an equal sign.

These commands set a value. The value follows the equal sign. For example, the following command will set the radius to 1.34 units:
        radius= 1.34

The following command will open the job with the filename of "Engrave serial number.job"
        open job= Engrave serial number

2) Commands without equal signs.

These commands do something, but they don't set values. For example, the following command duplicates the texture geometry that is active:
       duplicate

• Use ASCII 135 to separate lines of text, ie, ‡

The phrase "ASCII 135" represents the ASCII character #135, which is one of the characters that people used to make footnotes. It looks like this: ‡

Each command has to fit on one line. As with a typical CNC program, the invisible carriage return and linefeed characters are used to separate the commands from one another. If you want to engrave a paragraph, all of the text has to be on one line, and the way to do that is to separate each block of text in the paragraph with the ASCII character 135 to show MillWrite where a block of text ends. For example, to engrave these three lines:
    Part 5501-a
    SN: 123
    Made in USA

Put that footnote character at the end of each line like this:
    engrave= Part 5501-a‡SN: 123‡Made in USA
   
You don't need to put a footnote character at the very end of the text.   

Here are the commands that MillWrite has right now.

   • *             The * is a comment for yourself, MillWrite ignores it
                     Don't put a comment on a line that has text or MillWrite will assume it's part of the text.
                     It is best to put the comment on a line by itself.
   • countersink depth=
   • countersink num=
   • duplicate
   • engrave=             use ASCII 135 to identify the end of each line of  text
   • feed=
   • line length=
   • polyline               followed by x, and y values,  and optional z, values
   • machining batch=
   • machining order=
   • max depth per cut=
   • move to xy=
   • open job=
   • radius=
   • replace text=           use ASCII 135 to identify the end of each line of  text
   • rotate=
   • scale xyz=
   • speed=
   • surface radius=         the radius of the cyclinder , which may be on a 4th axis
   • surface z=        
   • tap depth=
   • tap num=
   • text align=           
   • text angle=
   • text height=
   • text length=
   • text height and length=
   • tool depth=
   • tool diameter=
   • tool num=
   • tool z surface=
   • use item=               followed by the text name of the item to activate
   • work offset=            eg, G54, G55, etc
   • x=
   • y=

   • edit group                           for editing a "grouping"
   • finished with group

   • save cnc=
   • transmit cnc=

   • apply tool table
   • disable 4th                    
   • read tool text file=           ie, get tools from tool list.txt
   • remove unused
   • reorder                          reorder machining order to reduce rapid moves

   • make datamatrix=       creates a Data Matrix barcode
   • cell size=                       only for Data Matrix barcodes

Some commands need to be placed in a certain order in order for them to work properly, but some commands can be placed anywhere because they are merely instructions to MillWrite. For example, the command to save the CNC file ("save cnc=") can be placed anywhere because it is simply telling MillWrite that you want the CNC program saved on disk. Example:

   save cnc= c:\NC Programs\engrave part number.cnc

That command does not modify anything, so it doesn't matter where in the command file you tell MillWrite that you want the CNC program saved.

However, some commands modify geometry or text, and that requires that they be placed after the text or geometry has been made "active". If you are creating new text and geometry, an item becomes active as soon as you create it, and it remains active until you create some other item.

For example, the command to create some text is "engrave=". After the text has been created, you can use any of the text or tool modification commands to adjust that text. It doesn't matter what order those other commands are in because all of them operate on the active tax. Both of the following sets of commands will do exactly the same thing:

   engrave= Part # 12-44 revB     this creates the text and makes it active
   text height= .25               it doesn't matter what order these other commands are in,
   tool depth= 0.034              as long as they are after the "engrave=" command
   tool num= 4

   engrave= Part # 12-44 revB
   tool depth= 0.034
   tool num= 4
   text height= .25

MillWrite has the ability to process the commands that people have requested, but there are hundreds of possible commands that MillWrite could process. Therefore, if you need a particular feature, add for it, and it will be add it to command list, assuming it is practical to do so.

Note that after the = you can put one or more blank spaces to make it easier to read.

   • open job=

This command will open a job and allow you to make modifications to it. Although it should be obvious, this should be one of the very first commands in the command file because in order to modify an existing job, you must first open it.
   • You do not need to include the extension ".job".
   • If you do not include a drive and folder, MillWrite will use whatever drive and folder that you specified to be the default folder for for job files (you set that at the Setup page).

You need to use this command when you want to open an existing job and modify one of the items within it.

A text item is identified by its text, and rectangles, polylines, and other items are identified by the "name" that you have given the item. In case you have not noticed, most of the items that you create have a "name" data field that is you have probably left blank. If you want to modify any of those items with a command file, you must give that item a unique name.

For an example of how to use this command, assume you created a job file that engraves a part number, serial number, and recycling symbol, and assume that you want to change the serial number each time. In that case, you might set up the serial number as "serial number", or as "replace this text". You could modify that serial number simply by making it active with the following command:

   use item= serial number
   replace text= SN 0034-3

Or:

   use item= replace this text
   replace text= SN 0034-3

Note: you don't have to specify the complete text, or the complete name, of the item. You only have to enter as much text as is unique. For example, assume you have these two lines of text in your job file: 

replace this text to engrave part number
replace this text for serial number

You can make the first text item active with any of the following four commands:

   use item= replace this text to engrave part number
   use item= replace this text to engrave part
   use item= replace this text to engrave
   use item= replace this text to

And you can make the second text item active with any of these three commands:

   use item= replace this text for serial number
   use item= replace this text for serial
   use item= replace this text for

Normally you use this command to replace the text that you want to engrave. It will also change the name of a polyline, rectangle, or other item, if you want to do something more complicated (an example of a more complicated use will be mentioned farther down in this document).

Note: each command can be only one line long. Therefore, if you want to replace a text item with multiple lines of text, you need to separate each line of text with an ASCII 135 character to let MillWrite know that each where to put the line breaks. For example, assume that you want to replace the text to engrave with the following paragraph:

    Do not put in dishwasher.
    Do not immerse.
    Part number 355-3
    Made in USA.

Use the ASCII character 135 to separate the lines, like this:

   replace text= Do not put in dishwasher.‡Do not immerse.‡Part number 355-3‡Made in USA.

This will change only the X coordinate of the active item. Example:
    x= 3.456

This will change only the Y coordinate of the active item.

This will set both the X and Y coordinates of the active item with just one commmand. Separate the X and Y values with a comma, tab, or a blank space. Example:
    move to xy= 3.456, -7.654

This will set the height of the active text. See the blue note below.

This will set the length of the active text. See the blue note below.

This will set both the height and length of the text and adjust the width ratio so that the text fits that particular height and length.  

Note about setting the text height and length:

Text has a height, length, and with ratio. You can set only two of those three parameters because the third is calculated from the other two.

If you are creating new text, it will be given a width ratio of 1.0. If you set the height of the text, the length will be adjusted in order to keep the width ratio at 1.0. If you set the length, then the height will be adjusted. If you want to set both height and length, then use the "text height and length= command.

However, if you are modifying a text item in an existing job file, and if the existing text already has a width ratio other than 1.0, then if you use the "text height= or "text length= commands, MillWrite will assume that you are trying to force the text to be a certain height and length, and so it will allow the width ratio to change.

To summarize this, when you create a job file that you plan to modify with a command list, and when you want to modify the text items in that job file, set their width ratio to 1.0 if you want the width ratio to remain 1.0 after you have modified them. If you modify a text item that has a width ratio other than 1.0, MillWrite will assume you are trying to force the text to fit a certain whatever height and length that you designed for that particular text item.

If you want the text to fit a certain height and length, The best option would probably be to use the command: "text height and length="

This will set the rotation angle of the text. Enter a value in degrees. The 3 o'clock position is at 0°, and the 12 o'clock position is at 90°.

If you want to set the alignment for the text, specify a value from 1 to 9. MillWrite offers nine alignment points for text. The XY coordinates of the text refer to the alignment point. For example, the following commands set the upper left corner of the text to be at a coordinate of 4.5, 7.3:

   use item= replace this text
   replace text= Part #: 56900 -rev2
   text height= .25
   text align= 1
   move to xy= 4.5, 7.3

This will set the feed rate of the tool for the active item.

This will set the speed of the tool in RPM for the active item.

This specifies the depth for the tool for the active item. The value is always positive. For example, the following command will set the tool to a depth of 0.5 units below whatever the surface is.

   tool depth= 0.5

This sets the tool diameter of the active item.

When you are engraving geometry, you do not need to specify the tool diameter because it has no effect on the CNC program. However, when you are contouring or pocketing geometry, the tool diameter is critical. Also, when MillWrite engraves text, it separates the characters by the width of the tool so that they don't cut into one another.

This will specify the tool number for the active item. This will become the "T" number in the CNC program.

This sets the Z coordinate at which the tool would touch the surface for the active geometry. It sets the data field that MillWrite refers to as "Z Surface"

This will set the max depth per cut of the tool for the active item.

This will set the machining batch of the active item.

This will set the machining order of the active item.

This command will duplicate, that is, make a copy, of whatever item is active. This command is useful when you need to engrave or cut several, nearly-identical items. You only have to create one item, and then you can duplicate that one item, and make changes to it.

For example, assume you need to engrave text at various openings on a mold. Some molds have to be engraved at five different locations, and others have to be engraved at six locations, and others need to be engraved at eight locations. You could create a job file for every possible situation, but if you have dozens of possible situations, that would be a lot of work.

It would be easier to create just one text file with just one text item. You would then activate that one text item, put it into the proper XY location, and then duplicate it for the second location. You would then change its XY coordinates, its text, and whatever else is necessary, and then you could duplicate it again.

The following set of commands will modify the text item that is called "replace this text". It will change that text to "Main Power", and then duplicate that item. The duplicate item will be moved to an XY coordinate of 1.23, 4.5, and the text will be replaced with ON/OFF. Then that text item will be duplicated, and the x-coordinate will remain what it already is, but the Y will be changed to 7.44, and the text will be replaced with "Fuel Level".

   use item= replace this text
   replace text= Main Power
   duplicate
   replace text= ON/OFF
   move to xy= 1.23, 4.5
   duplicate
   y= 7.44
   replace text= Fuel Level

This will rotate the active item by whatever degrees number of degrees you specify. The rotation is anti-clockwise if the value is positive, and clockwise if you enter a negative value. For example, the following command will rotate the item by 20° anti-clockwise.
   rotate= 20

When engraving text, you do not need to use this command. Text has a special command, "text angle=, which lets you specify the rotation angle of the text.

This will scale the active item by the X, Y, and Z values that you specify.

When you are engraving text, you normally will not want to use the scale command because you can more easily control the size of the text by setting the text height, and/or the text length. However, when the text is wrapped around a circular arc, or following a polyline, you might want to use the scale command.

Normally you will not want to scale in the Z axis, so you mormally would enter only one or two values, or specify a Z scaling factor of zero. If the scaling factor in Y is the same as in X, which is usually what you want to do, then you only need to enter one value. For example, the following command will scale the active item by a factor of three.
    scale xyz= 3

That is equivalent to this command:
    scale xyz= 3, 3, 0

If you specify an X scaling factor that is different from the Y scaling factor, then the item will be stretched or compressed. For example, the following command will stretch the item 3 times in the x-axis, but only two times in the Y axis.   
    scale xyz= 3, 2

If you wonder why somebody would want to scale an item differently in X and Y, one purpose is to make rectangles. For example, you could create a job file that has a square that is one unit in size. Then, whenever you want to cut a rectangle, the scaling factor becomes the size of the rectangle. For example, if you want to cut a rectangle that is 5 units in X and 7.6 units in Y, you would enter:

    use item= 1 unit square
    move to xy= 1.23, 4.5
    scale xyz= 5, 7.6
   
If you are scaling a circle, the scaling occurs from the center of the circle. If you are scaling something else, it occurs from wherever the start node is. Likewise, when you use the "move to xy= command, if you are moving a circle, it moves from its center, otherwise it moves from its start node.

If you want to create a new text item, rather than use some existing text, then use this command. As with the "replace= command, if you want to create a text item with multiple lines, separate them with ASCII 135. For example, the following command creates one text item with two lines of text:

   engrave= This is new text.‡And this is the 2nd line.

If you want to create a polyline, use this command, and follow it with a set of XYZ coordinates. This is the only command that does not follow the rule that each command is on its own line. In this case, the command polyline is on its own line, but underneath it are sets of coordinates, one for each node of the polyline. For example, the following command list will create a triangle:
    polyline
    0,0
    6,0
    3,5
    0,0

The start node of the polyline is the first XY coordinate, which in this case is 0,0. If you do not specify Z values, they will be set to zero. This command can be useful if you need to engrave some lines, arrowheads, or other shapes.
 
If you specify Z values, you will create a 3D polyline, which will enable you to cut 3-D shapes.

After you create a polyline, you can duplicate it, move it, scale it, or rotate it.

A polyline can be a long chain of lines, arcs, and splines. If you create a polyline that is just one, single line, then you can use the "line length= command to set the length of that line. For example, you could create a horizontal line in a drawing, and refer to it as "horizontal line". Your command file could then set it to whatever length you want, and move it into whatever XY location you please. For example, the following command list will set it to a length of 5.6 units, and move it to 1.23, 4.5.

    use item= horizontal line
    move to xy= 1.23, 4.5
    line length=5.6

This sets the radius of a point or circle. If you are going to create CNC code, you do not need to set the radius of a point. However, if you are using the command file to create a job file that remains on the computer screen, then you might to give the points the radius of the drill so that you can by see their size.

    use item= contoured circle
    move to xy= 1.23, 4.5
    radius=6.9

When you are cutting a cylinder on a 4th axis, or a cylinder that is clamped into a vise, this sets the radius of that cylinder.

When specifying a cylinder, or other three-dimensional shape, which you normally do at the SETUP page, this is the Z coordinate at which the tool would touch the top of the 3-D shape.
Note: do not get command this mixed up with the "tool Z surface=. The "Surface z= command defines the block of material that you are cutting, which affects the entire job, whereas "tool Z surface= sets the tool for only one piece of geometry.

There will be only one "surface z= commands in a command file, but there may be as many "tool Z surface= commands as there are items to cut.

If you want to cut a data matrix barcode, this command sets the data for the barcode.
Examples:
   1) To cut a data matrix barcode that contains the data "Part # 123786", do this:
      make datamatrix= Part # 123786
   2) To cut a data matrix barcode that contains these 3 lines of data:

     Part # 123786"
     SN 43304-1"
     Made in USA"

     Use the footnote character ASCII 135 (‡) to show where you want a line break, like this:

      make datamatrix= Part # 123786‡SN 43304-1‡Made in USA

This command is valid only if you have made a data matrix barcode active, either by creating it with "make datamatrix=, or by selecting one from an existing job. This sets the distance between the cells of the barcode.  

If you have used MillWrite to create a plain text file of your tools, this command will read one of those lists into the tool table.

For example, this will set your tools to whatever is in the file "Engrave brass tools.txt"  

   read tool text file= Engrave brass tools.txt

To create a plain text file of your tools, switch to the Setup page of MillWrite, and then click your RIGHT mouse button over the tool list button. A menu will appear, and one of the options is to Write The Tool List To A Text File. If you use that feature, you can save one or more tool lists, and you can modify them, also. The "read tool text file= command will read whichever of those tool lists you specify after the equal sign.

This command will apply your default tool table to the items in the drawing.

Be careful about where you place the "apply tool table" command in the command file. That command applies the tool table immediately, so it affects only the items that have already been created, not the items that are created after this command.

If you use the "open job= command to modify an existing job file, then it would be useless to put the "apply tool table" before the "open job= command. Instead, place it afterwards so that after the job has been opened, the tool table is applied to everything in the job. You can then use the command file to modify whatever tool settings you want to change.

For example, the following commands will open an existing job called Engrave part number, and the next command will read Engrave brass tools.txt to create a tool list, and then that tool list will be applied to everything in the job. After the tool table has been applied, the tool depth for the engraved text called "replace this text" is overridden with a new value.

   open job= Engrave part number
   read tool text file= Engrave brass tools.txt
   apply tool table
   use item= replace this text
   tool depth= 0.034
   replace text= Part #: 56900 -rev2
   text height= .25
   text align= 1
   move to xy= 4.5, 7.3

If you put the "apply tool table" command at the end of the command list, then you can ensure that all of the items in the drawing have those default tools settings.

If you are creating a new job there is no sense in putting this command at the beginning of the command list because there will be nothing in the job file yet. In that case, you would put it at the end of the command list so that it sets everything that you create to the default tool settings.

This command tells MillWrite to set the cutting order of the items in the job to reduce rapid moves.

This command has an effect only when you are modifying an existing job. It does nothing when the command file is creating a new job.

When you modify an existing job file, there might be some situations in which you do not want all of the text in that job file to be engraved, or you do not want all of the drilling points to be drilled, or you do not want all of the geometry to be contoured, etc.. Rather than delete the items that you do not want to use, you can use this command, and it will delete everything that you have not made active.

For example, assume you have a job file that has a line of text to engrave, a logo to engrave, and a drilling point. The following command list will engrave the text, but delete the logo and the drilling point:

        save cnc= 1000.EIA
        remove unused
        open job= Engrave serial number
        use item= replace this text
        replace text= SN 0034-3

If you want to use the drilling point, then you have to make it active, even if you don't do anything to modify it. For example:

        save cnc= 1000.EIA
        remove unused
        open job= Engrave serial number
        use item= replace this text
        replace text= SN 0034-3
        use item= drill hole

If you specify this command, instead of saving the CNC program on disk, MillWrite will transmit the CNC program through the serial port to the CNC machine. This command is useful only when your computer is connected to the CNC machine through a serial port, and the machine is ready to receive.

MillWrite will use whatever serial port protocol you have specified in this command. For example, if you have two serial port protocols, one of them is referred to as "Centroid on COM1", then the following command will use that serial port specification to transmit the file:

   transmit cnc= Centroid on COM1

If you want to specify the work offset number, and G54 to G59, enter the value in this command. For example, if you want G56, use this command:
   work offset= 56
  
Note that you will not get the G54 to G59 command in the CNC program unless you specified that the postprocessor include a work offset number. To do that, you need to put a "W#" in the Starting Code block and/or the Tool Change block, of the postprocessor.

When using a 4th axis, this command will cut whatever is the active item by holding the 4th axis motionless, rather than by rotating the 4th axis.

This is the same as checking the box that says "Disable 4th axis for this item", which you find at the bottom of the Tool tab, it the data field called "More options".