Contact our corporate or local offices directly.
Parent page: PCB Design Objects
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. It can be user-defined text or a special type of string, referred to as a special string that can be used to display board or system information or the value of user parameters on the board.
Strings are available for placement in both PCB and PCB Library Editors. Use one of the following methods to place a string:
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:
Additional actions that can be performed during placement are:
This method of editing allows you to select a placed string object directly in the design space and change its location, rotation, orientation, and size.
When a comment object is selected, the following editing handles are available:
The following methods of non-graphical editing are available.
Properties page: String Properties
This method of editing uses the associated Text dialog and Properties panel mode to modify the properties of a String object.
During placement, the Text mode of the Properties panel can be accessed by pressing the Tab key. Once the String is placed, all options appear.
After placement, the Text dialog can be accessed by:
After placement, the Text mode of the Properties panel can be accessed in one of the following ways:
The Properties panel supports editing multiple objects, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry can be edited for all selected objects. If values of a property are different for objects in the selection, the appropriate field will be shown as an asterisk (
*) – a new property value will be applied to all selected objects.
A List panel allows you to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering – by using the applicable Filter panel, or the Find Similar Objects dialog – it enables the display of just those objects falling under the scope of the active filter – allowing you to target and edit multiple design objects with greater accuracy and efficiency.
While string objects can be used to place user-defined text on the current PCB layer, it is not only 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 project information that is to be displayed on the PCB at the time of output generation.
The special strings that are available in a PCB document come from a number of sources:
FileName= '.Pcb_File_Name_No_Path' : PrintDate = '.Print_Date'.
The following are the predefined, system-based special strings available for use on a PCB document:
.Application_BuildNumber– the version of the software in which the PCB is currently loaded. When generating Gerber output, use this string to record the software build on which the design was created.
.Arc_Count– the number of arcs on the PCB.
.Comment– the comment string for a component (placed on any layer in the library editor as part of the component footprint).
.Component_Count– the number of components on the PCB.
.ComputerName– the name of the computer on which the software is installed and running.
.Designator– the designator string for a component (placed on any layer in the library editor as part of the component footprint).
.Fill_Count– the number of fills on the PCB.
.Hole_Count– the number of drill holes on the PCB.
.Item– the Item that the generated data relates to (e.g.,
D-810-2000). The data will be used to build that item.
.ItemAndRevision– the item and specific revision of that Item that the generated data relates to in the format
<Item ID>-<Revision ID>(e.g.,
D-810-2000-01.A.1). The data will be used to build that specific revision of that particular item.
.ItemRevision– the specific revision of the Item that the generated data relates to (e.g.,
01.A.1). The data is stored in that Item Revision within the target server.
.ItemRevisionBase– the Base Level portion of an Item Revision's naming scheme (e.g.,
.ItemRevisionLevel1– the Level 1 portion of an Item Revision's naming scheme (e.g.,
.ItemRevisionLevel1AndBase– the Level 1 and Base Level portions of an Item Revision's naming scheme (e.g.,
.ItemRevisionLevel2– the Level 2 portion of an Item Revision's naming scheme (e.g.,
.ItemRevisionLevel2AndLevel1– the Level 2 and Level 1 portions of an Item Revision's naming scheme (e.g.,
.Layer_Name– the name of the layer on which the string is placed.
.Legend– a symbol legend for mechanical drill plots. This string is only valid when placed on the Drill Drawing layer. Note: this is a legacy feature; place a Drill Table object for more detailed drill information.
.ModifiedDate– the modified date stamp of the PCB; it is automatically populated. Example:
.ModifiedTime– the modified time stamp of the PCB; it is automatically populated.
.Net_Count– the total number of different nets on the PCB.
.Net_Names_On_Layer– the names of all nets on the specific layer. This string is only valid when placed on an internal plane layer.
.Pad_Count– the number of pads on the PCB.
.Pattern– the names of the component footprints used on the PCB.
.Pcb_File_Name– the path and file name of the PCB document.
.Pcb_File_Name_No_Path– the file name of the PCB document.
.PCBConfigurationName– the name of the data set from which the output has been generated as defined in the Release view (Project Releaser).
.Plot_File_Name– for generated Gerber output, this string identifies the file name of the Gerber plot file. For printed output, it identifies the layer depicted within the output. For ODB++ output, it identifies the name of the parent folder in which the files are stored.
.Poly_Count– the number of polygons on the PCB (consisting of polygon pours, internal planes and split planes).
.Print_Date– the date of printing/plotting.
.Print_Scale– the printing/plot scale factor.
.Print_Time– the time of printing/plotting.
.Printout_Name– the name of the printout.
.Project- project name.
.ProjectRev- project revision.
.SlotHole_Count– the number of slotted holes on the PCB.
.SquareHole_Count– the number of square holes on the PCB.
.String_Count– the number of strings on the PCB.
.Total_Thickness– the thickness of the board.
.Total_Thickness(Board Layer Stack)-the thickness of the board layer stack.
.Track_Count– the number of tracks on the PCB.
.VariantName- the variant of the design from which the output has been created.
.VersionControl_ProjFolderRevNumber– the current revision number of the project, which is incremented whenever a full commit of the project (i.e., including the project file) is performed. Version control must be used for this string to contain any information.
.VersionControl_RevNumber– the current revision number of the document. Version control must be used for this string to contain any information.
.Via_Count– the number of vias on the PCB.
The PCB Editor uses TrueType fonts for string objects. In addition, support is available for presenting text strings in Barcode format. Barcodes are commonly used to tag and identify PCBs, streamlining inventory tracking through use of automated scan-machines, for example. Choice of font is made from the Text mode of the Properties panel.
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.
To use a TrueType font, set the Font Type (in the Properties panel) to TrueType then choose a font type from the drop-down field in the Font region. Use the B (bold) and/or I (Italic) options to add emphasis to the text as required.
Enable the Inverted option to display the text as inverted, with additional controls for the size, justification, and size of the border around the text.
The PCB Editor – True Type Fonts page of the Preferences dialog provides options for embedding TrueType fonts when saving a design and for applying font substitution when loading a design. Embedding fonts is useful when text is required to be displayed in a font that may or may not be available on a target computer upon which the design is loaded. Font substitution enables the specification of a TrueType font to be used as a replacement when loading a design where fonts have not been embedded and where fonts may not be available on the computer upon which the design is currently loaded.
Three Stroke-based fonts are available – Default, Sans Serif and Serif. The Default style is a simple vector font that supports pen plotting and vector photo-plotting. The Sans Serif and Serif fonts are more complex and will slow down vector output generation, such as Gerber.
To use a Stroke-based font, enable the Stroke font option (in the Properties panel) and choose a font type from the drop-down field in the Font region.
The software provides the ability 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, set the Font Type field in the Properties panel to
BarCode then define the display options as required.
BarCode ISO Code 39 (US Dept of Defense standard) and Code 128 (global trade identification standard) are supported and the actual text string from which the barcode is derived also can be displayed by enabling the Show Text option.
By using a combination of barcode and inverted text strings along with fills, if necessary, a clear barcode area can be defined on a board with more information textually than would otherwise be afforded by just the originating barcode text.
Contact our corporate or local offices directly.