Связаться с нами
Связаться с нашими Представительствами напрямую
Draftsman is an alternate way to create the graphical documents for board design production. Based on a dedicated file format and set of drawing tools, the Draftsman drawing system provides an interactive approach to bringing together fabrication and assembly drawings with custom templates, annotations, dimensions, callouts, and notes.
The Draftsman PCB drawing capabilities are available through an Altium NEXUS Extension application, which is automatically installed with Altium NEXUS. The extension can be manually installed/removed or updated from Altium NEXUS's Extension & Updates page (DXP » Extensions and Updates). The Draftsman extension is located within the Installed tab and within the Updates tab when a software update is available.
The Draftsman drawing application can act as an adjunct, or even an alternative, to the production of graphical-type PCB production documents using traditional outputs. It offers automated placement of assembly and fabrication drawings on demand, and includes a wide range of manual drawing tools that can be used to add important details and highlighting to its multi-page documents.
The tool's key features include:
The Altium Draftsman application creates and saves PCB drawing files (
*.PCBDwf) and uses specific template formats for defining Sheet (page) properties (
*.DwsDot) and Document content (
*.DwfDot). The 'smart' document templates can be configured to automatically populate the document with nominated PCB drawing views and information text. When initially created, Document templates can use current Sheet templates to define the page properties (size, style, margins, etc.).
A new Draftsman document is created in Altium NEXUS using the File » New » Draftsman Document command. The New Draftsman Document dialog opens.
The dialog allows for the selection of a predefined Document Template (three are provided with the installation) or a Default option that creates a blank A4 document – note that a Sheet Template can be applied once the new document has been created. The button opens the Draftsman - Templates page of the Preferences dialog, where the location of the templates directory is defined.
Along with the desired Draftsman template, a specific Project and board Source Document can be selected where multiple files are open in Altium NEXUS. The new document will be associated with, and therefore draw data from, the nominated project, which will become the active project. The newly created document will be added to the nominated project.
PCB Draftsman files are a multi-sheet format, which allows documents to contain individual pages (sheets) that are assigned to particular types of board project production information. Sheets can be added to and removed from the current document with the Tools » Add Sheet and Tools » Remove Sheet commands (the commands are also available on the right-click context menu).
The currently active sheet number and the total number of sheets in a document are shown in the Status bar at the bottom of the workspace.
The page properties of a Draftsman document can be defined from the Sheet Properties dialog dialog (Tools » Sheet Properties or choose Sheet Properties from the right click menu).
The settings in the Sheet Properties dialog determine the base structure (size, border, settings, etc.) of the current page or all pages in the document. Alternatively, the page format can be defined by loading a (custom) sheet template document.
Select the dialog's Format & Size tab to access manual or template-based settings for the document's page size/content. The options are:
Use the Apply to selection to change the sheet settings for the active page (Current Page) or all pages in the document (Entire Document).
Select the dialog's Margins & Zones tab to access settings for the page border and its graphical divisions. The options are:
Use the Apply to selection to change the sheet settings for the active page (Current Page), or all pages in the document (Entire Document).
An Altium Draftsman document can use templates to define its page properties (Sheet template), and for new documents, a range of predetermined content (Document template). Both types of templates can be created from the PCB drawing file (file extension
PCBDwf) that is currently open in the editor by saving the document as one of the template types (
DwfDot). A Template document may be reopened, edited and saved to modify its content and properties.
Sheet (page) templates contain the graphics information for a page, including sheet sizes, parameters, and zones and border settings. Objects created with the editor's graphics tools (such as lines, rectangles, circles, and text) are also included – for example, a constructed Title block and content. A Sheet Template can be used to define the graphic format of a new or existing drawing document, and are also saved as part of a Document Template.
To save the current drawing document format as a Sheet Template, select the File » Save Copy As (or just Save As) command and choose Altium Draftsman Sheet Templates (*.DwsDot) from the save dialog's Save as type selection filter. Any elements that are incompatible with the Sheet Template format will be removed, such as placed drawings or additional pages. Before saving, an alert dialog will detail the pending action if incompatible elements exist.
Note that a saved Sheet Template can be applied to a Draftsman document page from its Sheet Properties dialog – select the dialog's button to locate and load a specific Sheet Template.
To save the current drawing document format as a Document Template, select the File » Save Copy As (or just Save As) command and choose Altium Draftsman Document Templates (*.DwfDot) from the save dialog's Save as type selection filter. All of an existing drawing document's content and attributes, with the exception to those that relate to data extracted from the PCB design, will be saved as a Document Template. If the source drawing document has a specific page style (as might be applied by a Sheet Template) these graphical elements and attributes will be saved with the new Document Template.
Any elements that are incompatible with the Document Template format will be removed. Before saving, an alert dialog will detail the pending action if incompatible elements exist.
A multi-page Draftsman document might typically contain assembly drawings, drill tables and drawings, layer stack and BOM tables, and fabrication drawings. When saved as a Document Template, the data from the current PCB is retained to define a drawing content 'shell'.
When subsequently used as a template for a new drawing document, the project's current PCB data is loaded into the shell in place of the template PCB data, therefore, recreating the document format and its type of content.
Both Sheet and Document templates can be opened as free documents in Altium NEXUS and edited accordingly. Open a template by selecting File » Open and choose Altium Draftsman Sheet Templates (*.DwsDot) or Altium Draftsman Document Templates (*.DwfDot) from the browser filter options.
An open Document Template will include the PCB design data that applied when the template was created, and also the Sheet Template properties that were active when it was created. If a Sheet Template defined the page properties in that Document template, it will need to be reapplied if the Sheet Template has changed in the interim.
The options settings for a PCB Draftsman document can be defined in the Draftsman Document Options dialog, which is accessed from the Tools » Document Options menu command. Note that the document options apply to the entire drawing document, however, the Sheet Properties settings apply to individual document sheets (pages). Both the Document Options and Sheet Properties are saved with the current Draftsman document.
The Draftsman Document Options dialog provides the following settings for the current Draftsman document:
The Altium Draftsman application allows a range of automated production drawings to be placed directly onto a Draftsman drawing document. The type of drawing to be placed is selected from the editor's Drawing Views icon collection, or by selecting a drawing type from the main Place menu.
When placed in the document, drawings can be manipulated within the page and their properties edited from a dedicated Draftsman Properties panel. If not already open, the panel can be activated by double-clicking on a placed drawing view, by selecting the drawing view and choosing Properties from the right-click option menu, or by clicking on the button at the bottom of the work area.
The panel provides editing access to the detailed properties of objects that have been placed in the drawing document. Select an object or view to see its properties in the panel.
A number of the panel sections (groups of options) are common to most of its view modes, as instigated by selecting drawing object. These are:
0.9would represent 90% (the Use Custom Scale option).
An Assembly view for the nominated project PCB is placed in a document with the Place » Board Assembly View command, or with the icon from the Drawing Views options.
The view shows the board outline with cutouts, holes, and component graphics with additional notation. The component graphics are automatically generated and take data on a priority basis from several sources:
A component's visibility, designator attributes and the geometry source (option 1, 2 or 3 above) used for forming its graphics can be changed in the Component Display Properties dialog, which is opened from the Draftsman Properties panel.
The Board Assembly View mode in the Draftsman Properties panel offers the following settings (use the button to expand/collapse option groups):
How components are displayed in an Assembly view is configured in the Component Display Properties dialog, which is available from the button in the Board Assembly View of the Properties panel.
Using the Show menu, the Component Display Properties dialog can be selected to display the component properties in different formats, with grouping choices of components, classes, footprints, and by BOM entry (the Footprints grouping is shown selected in the image below). The dialog allows control of the visibility and graphics for individual components and includes the following options:
.Designatorspecial string) on a specified Mechanical Layer.
To ease the task of locating and changing options for multiple entries, the Component Display Properties dialog also provides smart filtering capabilities, which can be activated from the icon in each column header. Select the desired entry in the filter drop down list to constrain (filter) the dialog contents to components that match the selected attribute. Multiple filter options can be applied and then disabled or cleared using the filter entry checkboxes in the dialog's lower border.
To create a more advanced or compound filter constraint, select the Custom option from the filter drop down list.
A Fabrication view for the nominated project PCB is placed in a document with the Place » Board Fabrication View command, or with the icon from the Drawing Views options.
With the placed fabrication graphic selected in the editor, the Board Fabrication View mode in the Properties panel offers the following settings:
The Drill Drawing view for the selected PCB is placed in a drawing document with the Place » Drill Drawing View command or with the icon from the Drawing Views options.
With a placed Drill Drawing graphic selected in the editor, the Drill Drawing View mode in the Properties panel offers the standard drawing view settings, such as Position, Title and View. The panel mode's additional properties settings are:
The Drill Symbol Configurations dialog presents a tabular view of PCB hole data, with hole styles grouped on a selectable parameter (column data) basis and assigned standard symbols. The dialog is activated by the button in the Properties panel, when in Drill Drawing View mode (as above).
The dialog's hole data table provides a flexible approach to assigning holes styles to Drill Drawing symbols, along with setting the symbol display graphics and sizes. By using the selectable hole parameters offered by the Grouping drop-down menu, the chosen criteria will group hole types under one symbol.
For example, in the above image the criteria is configured to group holes by Size, Plated status, and Tolerance, so all holes that have these parameter values in common are collected under the one drill symbol. By contrast, if the grouping criteria was set to 'Drill Layer Pair', all holes would be grouped under one symbol – since for this PCB, the parameter value applies to all holes (only one Drill Layer Pair is used in the PCB design).
The displayed Drill Symbol for a hole group, in both the Drill Drawing View and a placed Drill Table, is selected from the Symbol Graphics menu in the Drill Symbol Configurations dialog. The supported symbols include a range of graphic shapes and letter characters.
The Draftsman document Detail View feature allows a defined area of a drawing to be brought out to a floating, magnified view of its detail. The magnification factor (scale), labeling and line attributes of the detailed view can be configured in the Board Detail View mode of the Properties panel.
To place a Detailed View, select the Place » Board Detail View command or click the icon from the Drawing Views tools options. The placement procedure is as follows:
Detail Views may be added all graphical board views, including the Assembly View, Fabrication View, Section View, and Drill Drawing View.
A Section View provides a profile slice, or sectional, drawing taken from a nominated 'cut' point through a placed PCB Assembly View. The section view generator takes the available 3D data from the current PCB to create a standalone section drawing that is aligned to the nominated cut point. Any number of Section Views can be created from an Assembly View, and the section parameters may be modified after they are placed.
To begin the process of creating a Section View, use the Place » Board Sectional View command, or select the icon on the Drawing Views toolbar. The steps to create Section B-B shown in the following image would be:
A-A) will follow the cursor movement – use the Spacebar to toggle between vertical and horizontal cut lines.
The Board Section View mode in the Properties panel provides additional options for a selected Section View, such as its scale, label, style, and orientation.
A Draftsman document's Layer Stack Legend view provides a representation of the board's internal structure as an enlarged sectional view. It includes detailed descriptions and information for each layer in the stack, including the Gerber files associated with each layer.
By default, the information for each layer is derived from the corresponding attributes in the Board Layer Stack, as defined in the Layer Stack Manager dialog (Design » Layer Stack Manager in the board editor), however the layer description attributes may be edited and expanded through the Layer Stack Legend mode of the Properties panel.
To place a Layer Stack Legend view in a drawing document, use the Place » Layer Stack Legend command or select the Icon from the Drawing Views toolbar.
To configure how data is displayed in a Layer Stack view, access the Properties panel's Layer Stack Legend mode by double clicking on the placed view or selecting Properties from its right click options. The panel mode provides a comprehensive range of grouped attribute settings that allow for detailed fine tuning of a placed Layer Stack Legend view. Use the button to expand/collapse panel option groups.
The more important settings in this panel mode are:
The Layer Information dialog allows a large degree of control over the layer information displayed in the Layer Stack Legend view table. To open the dialog click the button under Settings in the Properties panel's Layer Stack Legend mode.
The Layer Information dialog allows the following editing options:
Altium Draftsman provides a range of additional drawing and annotation tools designed to add important information to a Draftsman drawing document. These include both automated note and highlighting systems plus free-form drawing capabilities. The dimension tools apply to a placed Assembly Drawing view and are available under the main Place menu or from their respective icons on the Drawing Annotations toolbar.
Object dimension graphics may be placed on an Assembly Drawing view to indicate the lengths, sizes, and angles of the object outlines, or the distance between nominated objects – dimensions may also be added to a Section View of an Assembly Drawing. To place a dimension graphic, select the desired type from the Place menu or from the Dimension drop down menu () on the toolbar.
A linear dimension can be added to the object's outline edge or between two object points. To place the dimension:
A dimension graphic can be moved after it has been placed, but only within its angular plane (horizontal, vertical, etc.). Most aspects of a placed dimension are available for editing in the dimension mode of the Properties panel – select a placed dimension to enable its associated panel mode.
Notable options that are available in the panel's Dimension mode are:
nom, respectively, would create
~10.5nomwhere the dimension value is
10.5. Text will show the unit name suffix, eg;
mm, when that option is enable in the panel's Units section.
A radial dimension can be added to a circular hole object on an Assembly Drawing. To place the dimension:
The Radial dimension measurement graphic can be moved (select and drag) or edited in a similar way to the Linear Dimension graphic. Again, most aspects of the placed dimension are available for editing in the Radial Dimension mode of the Properties panel – select a placed radial dimension to enable its associated panel mode.
An angular dimension can be added between two object edges on an Assembly Drawing. To place the dimension:
The Angular dimension measurement graphic can be moved (select and drag) or edited in a similar way to the Linear Dimension graphic. Most aspects of the placed dimension are available for editing in the Angular Dimension mode of the Properties panel – select a placed angular dimension to enable its associated panel mode.
Draftsman document Callouts can be placed on drawing views to provide further information on components and general objects, or on Assembly Drawing views, synchronized indicators for BOM entries and Note items. As such, the source text for a Callout can be a custom entry, a link to a specified Note entry, or an automated reference to a BOM item.
To place a Callout:
When placing a Callout, its type is automatically selected based on the selected source object, as follows:
To create a Note Item reference, or to change an existing Callout to another type, select the appropriate Source Type in the Source section of the Properties panel's Callout mode.
Draftsman document Note Item lists can be placed as free text entries in any location. The entries can be referenced by Callouts (see above) and both configured and edited in the Properties panel's Note mode.
To place a Note Item, select the Insert Note tool and then click to place the default Note entries in the drawing space. Select an entry in the list to edit its text content and number icon style in the Properties panel. Use the Add/Delete buttons to include and remove list entries, and configure the order of the text entries using the Up/Down buttons.
By way of example, to add a new Note entry that uses one of the preset document parameters:
A PCB Draftsman document allows both Bill Of Materials (BOM) and Drill symbol/data tables to be placed on the drawing and subsequently configured in the Properties panel. The tabular data is directly derived from the project PCB files and provides a simple, visual way to convey crucial information for the PCB fabrication and assembly processes.
The BOM/Drill placement options are available under the main Place menu or from their respective icons on the Drawing Annotations toolbar.
To place a BOM table, select the BOM table placement tool and click to position the table on the drawing document.
Select the placed table to enable the Bill of Materials mode of the Properties dialog, which provides configuration options for most aspects of the BOM table, including its visual attributes and data content. The Data Filtering options allow the BOM content to reflect a selected board design Variant (Variations), and/or filter the content to that of any Assembly View that has been placed on the document (the default is 'All' content).
Use the panel's Columns section to manage the table's data columns, however, the grouping and content of the columns will depend on how the BOM itself is configured, as outlined below.
Setup the BOM table's available content and data grouping in the Bill Of Materials Configurations dialog, which is opened from the button in the Properties panel under the Configurations section. The dialog provides the following BOM configuration options:
The Properties panel's Columns section allows the column order to be rearranged using the Up/Down buttons, columns to be removed (visually disabled) or new columns added. Use the button to include a new data column in the table – the next available data column is added with each click of the Add button. Use the button to reset the list of data Columns.
To place a Drill table, select the Drill Table placement tool and click to position the table on the drawing document.
Select the placed table to enable the Drill Table mode of the Properties dialog, which provides configuration options for most aspects of the Drill Table, including its visual attributes and data content (through Data Filtering and Column selection). Note that the panel's Units section allows for dimension entries (such as those in the Hole Size column) to be set to one or both of the available units (mm or mils), which also have individual Precision settings.
Use the panel's Columns section to manage the table data sort order, and column visibility and position order. The sort order buttons () toggle between off, ascending, and descending modes, and sorting can be applied to multiple columns.
The Drill Table's symbol styles, and the grouping of drill hole types under those symbols, is determined by the settings in the Drill Symbol Configurations dialog opened from the panel's button (under Drill Symbols). This is the same dialog that is activated from the panel when in Drill Drawing View mode, but in this case, only those columns activated (made visible) for the Drill Table will be shown – note that the two Drill Symbol Configuration dialogs versions are from the same source and therefore interact.
Draftsman provides a range of graphical element tools that can be used to place basic, free-form drawing elements in a document. The tools are accessed from the main Place menu or from the Graphical Tools drop down menu () on the Drawing Annotations toolbar.
Place a graphic element by clicking to position its first node and then again to place its second node, therefore determining its size – that is, the length for a line, the radius for a circle, the distance between opposite vertices for a rectangle or text box, or the dimensions of a placed image graphic. The nodes will snap to the nodes or guidelines of other objects, and optionally, the document snap grid if enabled.
See the Snapping tab in the Draftsman Document Options dialog for graphical primitives snap options.
Placed graphical elements can be moved by selecting and dragging, or when multiple elements are selected (Ctrl-shift + click, or by lassoing). Individual nodes can also be selected and moved. For more options, select a placed graphical element to enable its associated mode in the Draftsman Properties panel – note that the Text Box content is defined in the panel, and this can include document parameters.
Draftsman provides further graphical options through the import of standard DXF files, which are loaded into the drawing space from the File » Import from DXF menu command. Use the Windows file browser to select a
*.DWG file then configure the import options from the DXF Import Settings dialog that opens:
Draftsman documents may be printed or generated as output files in the same manner as Altium NEXUS's other graphics-based documents (Schematic, PCB, etc.). New Draftsman documents (once saved) are automatically added to the associated PCB project, and are therefore available to all normal document generation and printing processes.
To print the currently active drawing document, select File » Print from the main menu (or Ctrl+P) and select the print options in the normal way. For Draftsman documents, the print dialog includes a scalable print preview with page navigation selectors.
To export a drawing document to a single or multi=page PDF file (as determined by the document structure), select File » Export to PDF from the main menu.
A Draftsman drawing document is added to an OutJob by first opening an existing Output Job file or creating a new Output document (File » New » Output Job File).
To add a Draftsman document to the output job, select the Add New Documentation option under the Documentation Outputs section then select PCB Drawing. Assign the newly added output file (
*.PCBDwF) to a PDF output by selecting that container option and then checking the enable option associated with the Drawing document.
The Altium Draftsman PCB drawing capability is enabled in Altium NEXUS through the Draftsman software extension, which is automatically installed with Altium NEXUS – as is the case with other software extensions such as the Vault Explorer.
To manually install the extension, select the Purchased tab in the Extension Manager (DXP » Extensions and Updates) and locate the Draftsman extension. Click its download icon to download and install the extension then restart Altium NEXUS to enable the software's full functionality.
Once installed and ready to use, the extension will appear under the Extension Manager’s Installed tab. The Draftsman drawing features, including the ability to create a new Draftsman document file, become available when a Schematic or PCB project document is open.
The extension's preferences are available in the Draftsman section of Altium NEXUS's Preferences dialog (DXP » Preferences).
The Draftsman - Primitives Defaults page of the Preferences dialog allows the default values and settings to be configured for drawing and objects placed in a Draftsman document. These default settings can be overridden in the Draftsman Properties panel once an object or view has been placed in a document.
The Draftsman - Templates page of the Preferences dialog is used to define the location of Draftsman Sheet and Document templates.
Связаться с нашими Представительствами напрямую
Пожалуйста, заполните форму ниже, чтобы получить ценовое предложение.
Если Ваша подписка Altium активна, у Вас нет необходимости в пробной лицензии.
Если у Вас нет активной подписки Altium, пожалуйста, заполните форму ниже, чтобы получить пробную версию.
Вы нашли нужное место! Пожалуйста, заполните форму ниже, чтобы начать использование пробной версии.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.
Вы можете загрузить бесплатную лицензию средства просмотра Altium Designer Viewer сроком действия 6 месяцев.
Пожалуйста, заполните форму ниже, чтобы запросить эту лицензию.
Замечательно! Создавать новое - отличное занятие. У нас есть превосходная программа для Вас.
Upverter - бесплатная платформа, разработанная специально для любителей проектирования.
Нажмите здесь, чтобы попробовать!
Вы можете загрузить бесплатную лицензию средства просмотра Altium Designer Viewer сроком действия 6 месяцев.
Пожалуйста, заполните форму ниже, чтобы запросить эту лицензию.