PCB_Cmd-PlaceStringPlaceString_AD

Applied Parameters: None

Summary

This command is used to place a String object onto the active document. A string is a primitive design object. It places text on the selected layer in a variety of display styles and formats, including popular barcoding standards. As well as user-defined text, a special type of string, referred to as a special string, can be used to display board or system information, or the value of user-parameters, on the board.

In addition, true multi-line text support simplifies the task of adding substantial sections of text into PCB layouts, such as that often included to provide technical, mechanical, and assembly notes, on board mechanical layers.

Access

Strings are available for placement in both PCB and PCB Library Editors:

• PCB Editor - the following methods of access are available:
  • Choose Place » String from the main menus.
  • Click the  button on the Wiring toolbar.
• PCB Library Editor - the following methods of access are available:
  • Choose Place » String from the main menus.
  • Click the  button on the PCB Lib Placement toolbar.
  • Right-click in the workspace and select Place » String from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter string placement mode. A string will appear "floating" on the cursor:

1. Position the cursor and click or press Enter to place a string.
2. Continue placing further strings, or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

• Press the Spacebar to rotate the string anti-clockwise, or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step, defined on the PCB Editor – General page of the Preferences dialog.
• Press the X or Y keys to mirror the string along the X-axis or Y-axis respectively.
• Press the L key to flip the string to the other side of the board.
• Press the + and - keys (on the numeric keypad) to cycle forward and backward through all visible layers in the design respectively – to change placement layer quickly.
• Press the Tab key to access the String dialog, from where properties for the string can be changed on-the-fly.

Tips

1. The default text for a newly-placed string object is String. Once placed (unless changed before or during placement), change this text as required using the text entry window in the String dialog. Dynamic word wrapping allows text to be entered as needed, automatically wrapping to the next lines as needed. Forced line breaks (carriage return + line feed characters) can be inserted by simply pressing the Enter key while entering text. Forcing a break to a new line allows a multi-paragraph formatting approach, if required.
2. While string objects can be used to place user-defined text on the current PCB layer, it's not just user-defined text that can be placed. To assist in producing documentation, the concept of "special strings" is used. These act as placeholders for design, system or user information that is to be displayed on the PCB at the time of output generation:
   1. A special string is denoted by the string starting with a . (dot) character (e.g. .Layer_Name, .Net_Count, etc).  If a string starts with ".", the entire string is treated as a 'special' string. This syntax is also used when referencing a user-parameter, the parameter name is preceeded by the . (dot) character.
   2. There is a default set of predefined special strings provided for use with new PCB documents. The designer can also add their own custom special strings, by defining additional parameters at the project-level, these parameters are defined in the Parameters Tab of the Options for Project dialog.
   3. To include more than one string in a 'special' string, use apostrophe ( ' ) to enclose each string. Example:  '.PcbDoc' '.PcbName'.
   4. Spaces and/or special characters can also be used inside 'special' strings. Example: '.PcbDoc #1'.
   5. To use a special string on a PCB, simply place a string object and enter the special string name in the text entry window of the associated String dialog. As you start to type the name of the special string (including the dot prefix), a list of matching special strings will pop-up, from which to choose.
   6. The values of some special strings can only be viewed when the relevant output is generated. Most special strings can be viewed directly on-screen however, by enabling the Convert Special Strings option, on the View Options tab of the View Configurations dialog, when viewing the board in 2D (press the L shortcut to open the dialog).
3. Three Stroke-based fonts are available – Default, Sans Serif and Serif. The Default style is a simple vector font which supports pen plotting and vector photoplotting. The Sans Serif and Serif fonts are more complex, and will slow down vector output generation, such as Gerber.
4. When using TrueType fonts, TrueType and OpenType (a superset of TrueType) fonts found in the \Windows\Fonts folder will be available for use. The feature also offers full Unicode support. Note that only detected (and uniquely named) root fonts will be available for use. For example, Arial and Arial Black would be available but Arial Bold, Arial Bold Italic, would not.
5. Ability is provided to place barcode symbols directly onto a PCB on any layer, allowing barcodes to be easily imprinted on a PCB as part of the manufacturing process. To use a Barcode font, simply set the Font field (in the String dialog) to BarCode, and define the display options as required in the Select BarCode Text region. BarCode ISO Code 39 (US Dept of Defense standard) and Code 128 (global trade identification standard) are supported, and the actual text string that the barcode is derived from can also be displayed.