Contact our corporate or local offices directly.
Draftsman is an alternative 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 Designer Extension application, which is automatically installed with Altium Designer. The extension can be manually installed/removed or updated from the Altium Designer Extensions & Updates page (select the Extensions and Updates option from the system User menu – ). 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 Designer using the File » New » Draftsman Document command. The New 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 Designer. 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 settings for individual pages (sheets) in a Draftsman document can be defined in the Properties panel, under the Page Options tab.
Open the Properties panel from the system button, or select View » Panels » Properties from the main menu. The panel’s Document Options mode is active when no object is selected in the workspace.
The settings under the Page Options tab determine the base structure (size, margins, etc.) of the current page or all pages in the document. Alternatively, the page format can be defined as a custom size, or by loading a sheet Template document.
Changes made to the Page Options properties can be applied to the current page (), or all pages in the document (). For settings that apply to the overall Draftsman document and its constituent pages, see Document Options below.
► See the Properties panel Page Options section for more information.
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 the Properties panel Template section under the Page Options tab – select the option and click the 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 Designer 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 settings for the overall Draftsman document (potentially composed of multiple sheets/pages) are defined in the Properties panel, under the General tab.
If not already active, open the Properties panel from the system button, or select View » Panels » Properties from the main menu. The panel’s Document Options mode is active when no object is selected in the workspace.
The Document Options settings determine the document’s source design data, graphic styling, drawing behavior and the applied units. Changes to the settings override the panel’s default property settings, which are defined by current document template – such as the default template (
► See the Properties panel Document Options Mode for more information.
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 icons presented in the editor's Active Bar (located at the top of the workspace) or the Drawing Views toolbar. Alternatively, a drawing type can be placed from using main Place menu or by right clicking in the workspace and selecting a Place option from the context 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 selecting the Properties option from the system menu.
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 Draftsman Board Assembly View is an automated graphic composite of the active PCB project's board outline, cutouts, holes, and component graphics with additional notation. An Assembly View for the nominated source project PCB is placed in a document by selecting the object icon, or via the Place menu options.
The Board Assembly View's component graphics are automatically generated and take data on a priority basis from several sources, such as:
A component graphic on a nominated board mechanical layer (used as a design assembly layer) – the layers used are specified in the Source section of the Properties panel in Document Options mode.
Note that the automatic generation of a Board Assembly View does not rely on the availability of an additional board assembly layer (for example, Top/Bottom Assembly), so this mode is an option.
A component's visibility, designator attributes and the geometry source options used for forming its graphics can be changed in the Component Display Properties dialog, which is opened from the button in the Draftsman Properties panel. The graphic properties for all components in the Assembly View are available.
Alternatively, when a component is selected on the Assembly Drawing itself, that component's graphic configuration options become available in the Component Display Properties section of the Properties panel.
► See Board Assembly View Properties for information on the property settings available for an Assembly View.
How individual 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 selected in the example images). The dialog offers a Geometry tab view for configuring how components are drawn, and a Parameters tab to specify the component information that will be is shown.
The Component Display Properties dialog's Geometry tab view allows control of the visibility and graphics for individual components, and includes the following options:
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.
The Component Display Properties dialog's Parameters tab view allows control of the visibility and positioning of both Designators and Custom Parameters for the named components. It includes the following options:
.Designatorspecial string) on a specified Mechanical Layer.
Select the Add Parameter button () to add another set of Parameter columns in the dialog –
In the example Parameter addition shown in the image above, a custom component Parameter named
Internal Component Ref has been added, and its Location and Font specified. The component's Designator has been set to a larger font and positioned at the center of the the component graphic.
Draftsman also includes direct, manual component Designator control and positioning. This adds to the capabilities available in the Component Display Properties feature by providing direct control through the Properties panel of the positioning, sizing and style for individual designators, or designators on a BOM item basis. Also, designators may be manually positioned in the drawing space by a simple drag and drop process.
The immediate control of designators is accessed from the Component Display Properties section in the Properties panel, which is enabled when a component or its designator is selected in a placed Assembly view. For the selected component, the designator properties are equivalent to those for its specific component entry in the Component Display Properties dialog – opened by selecting the button in the panel’s View section.
Changes made in the panel’s Component Display Properties will affect the currently selected component in the drawing view. To change the properties for all components of that type, check the Apply changes to all instances of same BOM option. This will detect the component’s BOM item entry and propagate the property change to all those components.
For example, to modify the display properties for all
0.1uF capacitors with the
CC2012-0805 footprint (the BOM entry for a selected bypass capacitor), select the Apply changes to all instances of same BOM option and then make the component display property change. This is equivalent to locating and changing the properties of the BOM entry in the Component Display Properties dialog.
For direct free-form placement of a component dialog, simply press Ctrl while selecting the designator in the workspace and then drag it to a new location. Press the space bar to rotate the designator by 90° steps while you drag. Note that its Designator Location setting in the Properties panel will change to Manual.
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 standard Isometric Projection view for the currently specified PCB can be placed in a document with the Place » Board Isometric View command.
The properties and options for a placed Isometric View are edited from the Properties panel, which will change to its Board Isometric View mode when the view graphic is selected in the workspace. Use the panel's View – Face Side drop down menu to select the projection view perspective, and the Variants menu to specify which project design variation (if available) is shown.
In the above images (drawing document and Properties panel), the placed Front side view is set to the
SL1 Supply option 1 Variant, which has one of the voltage regulator devices marked as 'not fitted'.
If the Properties panel is not already open, it 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.
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:
Controlled Depth Drilling (Backdrilling) in Altium Designer is a methodology for detecting and removing electrically redundant sections of plated through holes.
These are typically found where a standard through-hole Via connects the signal to an inner layer, leaving the remaining portion of the Via barrel as an undesired ‘stub’ – in turn, this stub is likely to compromise the performance of a high speed design. In the backdrilling technique, the stubs are removed by drilling to a precise (Z) depth with a slightly oversized drill.
Altium Designer uses a specific Design Rule and assigned Back Drill Pairs to automatically create the correct NC Drill output files. In a Draftsman document this arrangement is represented in the Layer Stack Legend, which now includes a graphical representation of all Drill Pairs defined for the board, including any Back Drill Pairs (shown with partially drilled out Via barrels).
Draftsman includes the capability to place and configure industry standard Geometric Dimensioning and Geometric Tolerances symbolic elements that define the manufacturing properties of objects included in a drawing.
Also used in most advanced MCAD applications, the specialized information provided by the placed geometric symbols stipulate the allowable imperfections in the manufacture of physical objects. The geometric definition elements that can be added to Draftsman documents are derived from standards developed by the American Society of Mechanical Engineers (ASME) – specifically, the ASME Y14.5-2009 Dimension and Tolerancing standard. Many other standards and guidelines exist for geometric engineering definitions, including a large number of conceptually specific documents from the International Organization for Standardization (ISO).
– See Geometric dimensioning and tolerancing for overview information and reference links.
In terms of Draftsman engineering documents, the symbol-based Dimensioning and Tolerancing information is incorporated into a drawing by the placement of two types of objects:
Both of the above drawing objects can be positioned freely in the document, or (normally) attached to a feature such as an edge. In the same way in which other Drawing Annotations are placed in Draftsman, such as Surface Finish symbols, the geometric definition symbols are attached by clicking on a highlighted line in the drawing and then clicking again to place the symbol.
Place a Datum Feature on a drawing using the Place » Datum Feature menu command or by selecting the icon from the Drawing Annotation toolbar, and attach it to a drawing feature as outlined above. The attached Datum element simply identifies that feature, such as an edge, as a reference on that drawing object.
The Datum Feature is identified by its Label entry in the Properties panel, so that relative dimension tolerances included in Feature Control Frames (see below) can refer to this and other placed datum.
Place a Feature Control Frame on a drawing using the Place » Feature Control Frame menu command or by selecting the icon from the Drawing Annotation toolbar, and attach it to a drawing feature as outlined above, or place it free space.
The information it conveys, presented in symbols, modifiers and numeric values, is entered in the Properties panel.
A Feature Control Frame offers symbol options and large number of elements that can be attached to specify manufacturing tolerances and constraints. Attached machining tolerances, such as the 'straightness' of a feature for example, apply to the specified drawing object face. Attached Dimension tolerances by comparison (such as 'position') are generally specified as relative to one or more placed Datum.
When added to the mechanical elements in a Draftsman drawing view, the combined information represented by Feature Control Frames and their related Datum references can fully describe the acceptable manufacturing constraints for that physical element.
In the example drawing view shown below, dimensions have been added, Datum Feature references attached to the three visible board edges, and Feature Control Frames applied to the top edge and two mounting holes. The Feature Control Frames have multiple elements added, which appear as a sequence of (selectable) rows – note the Add, Delete etc buttons in the Selected Element area of the Properties panel.
The symbols and formatting used in the various Feature Control Frames is fully described in the ASME standard, however an overview of the examples shown above is as follows:
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.
Ordinate dimensions are a neat and efficient way to add multiple drawing measurements that are all based on a single reference point. With this approach, the indicated dimensions are effectively cumulative as they are placed at increasing distances from the nominated reference point – the dimensions are relative to the origin point.
To place an Ordinate dimension object select Ordinate Dimensions () from the main Place menu or from the Dimensions dropdown menu, or select the command after right-clicking in the drawing workspace. The first location selected is the base coordinate that acts as the reference for the subsequent dimension points.
To create the series of dimension points:
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.
A further Callout Source Type data option is applying a Component Parameter from the board design. When selected, the Component Parameter source can be set to specify one of the available parameters for the Component selected by the Callout, as extracted from the Assembly View's source PCB document. Use the Properties panel Parameter drop down menu to nominate the displayed Parameter data.
Draftsman allows the placement of Surface Finish graphical symbols and their associated parameters that comply with the ISO 1302:2002 International Standard for surface texture in technical product documentation. The standard specifies the rules for the indication of surface texture in drawings, based on special symbols and attributes that describe the permitted surface material for the product – in this case, a printed circuit board.
The addition of Surface Finish indicators in Draftsman avoids the need for a separate Surface Finish tool or application when this standardized information is required for PCB manufacture. The graphical symbols are accompanied by a range specialized text codes, as defined by the ISO standard, that are added via the Draftsman Properties panel when a placed Surface Material object is selected.
To place a Surface Material symbol in a drawing, select Place » Surface Finish from the main menu, and then locate the symbol where it is associated with the board surface. Attach the symbol to a drawing by clicking on a highlighted line and then clicking again to place the symbol. The attached surface indicator can be dragged along the line, and optionally, away from the drawing via an automatic Extension Line. Select the With Leader option in the Properties panel to position the symbol away from the surface.
In most cases only one or two surfaces need to be defined, such as the surface of the top and bottom layers, so a minimal number of symbols/attributes are usually required. However, the indicators may be applied to the face of any engineered object, including the surfaces of rendered components.
The style of the Surface Finish symbol itself indicates the allowed processing of the surface material, as follows:
The string-based parameters (attributes) that are associated with the symbol indicate a range of manufacturing options, as defined by the standard:
– See the ISO Geometrical Product Specifications page for more information about the
ISO 1302:2002 standard.
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 Bill Of Materials (BOM), Tables, 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/Table 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.
The Bill of Materials (BOM) document for most advanced PCB projects tends to have a large number of entries, which can be difficult to recreate as a table that will fit into a drawing document. Rather than resorting to font and table scaling, multiple custom table entries or an external document, the Split BOM capability in the Properties panel allows a BOM Table to be presented over a number of 'Pages'.
To create the multiple BOM Pages, select a placed BOM (which is likely to exceed the document Sheet height) and check the Limit Page Height box in the Properties panel’s Pages section. This will restrict the height of the BOM table to the nominated height entry (Max Page Height, mm), and therefore the number of lines shown in the BOM table.
Draftsman detects that the entire BOM is not shown, as indicated by the panel's Page entry (for example,
1 from 2), and the associated drop down menu allows you to nominate which Page is shown. To add further Pages of the BOM, place another BOM (Place » Bill of Materials) and specify the next page under Page in the Pages section of the Properties panel.
Since each Page of the BOM is placed by adding another BOM table, and then configuring it accordingly, the individual BOM Pages (sections) can be placed on any Sheet in a Draftsman document. To place another, different set of split BOM Pages, specify an alternative BOM Table ID on a placed BOM – say,
1 rather than
A Draftsman document allows a generic Table to be placed on the drawing and subsequently configured in the Properties panel, and in the table cells themselves. The layout and content of the custom Table is free to be defined as required by its intended purpose, and offers a flexible way to include additional information in any Draftsman document.
The new Table is placed from the main menu (Place » Table), or from its icon on the Table menu in the Drawing Annotations toolbar. Use the following Insert Table dialog to nominate the initial number of rows and columns in the new Table, and therefore its number of cells.
Click to place the new Table attached to the cursor. Select the table and then use its positioning icon to change the table location.
The selected table will change the Properties Panel to its Table mode where the table's Title, Border and Cell Properties can be configured to suit.
Along with the Border line styles, for the table perimeter (Outer Line) and cell divisions (Inner Line), the style of individual Cell Properties (Width, Color, Padding and Text style) can be changed as required. Multiple cells can be selected to change their collective properties – use standard Shift-Click techniques, or click and drag across cells.
Right click in a cell and select the Table menu from the context menu to access the cell configuration commands. These provide a full set of Table manipulation functions for adding and removing Columns/Rows and Merging Cells.
By using both the Table commands and the options available in the Table Properties dialog, a custom Table can be created to suit a wide range of information needs in a Draftsman document. The Table shown below, for example, has been constructed to show the information taken from a board Stack Report.
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.
The background style for primitive drawing objects such as Rectangles and Circles can be set to solid or hatched ANSI-style fills. For these drawing objects, the color options for the solid and hatch patterns are definable via the Properties panel, and can be set to suitable defaults in the Draftsman Preferences page under their respective primitive entries (Drawing Tools – Rectangle and Circle).
To change a Circle or Rectangle shape’s background style, select it in the workspace and then click the Background browse button () in the Properties panel to open the Fill Style dialog. The selections include the solid/hatch options, the colors applied and the hatch pattern configuration.
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 other graphics-based documents in Altium Designer (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.
Print or Export to PDF
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.
Add to OutJob
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.
Altium Designer has the ability to create variations of a board design (Variants) and pass pass this variant information on to Draftsman, which in turn allows a design variation to be applied to a placed drawing View.
Project Variants are added in the project's Variant Management dialog, which also allows Parameters to be added to each variant. These parameters are typically applied as special (interpreted) strings in Altium Designer documents to indicate which Variant is currently enabled.
In Draftsman, a project’s current variant selection is made from the Variant menu in the in the View region of the Properties panel, which causes the placed view (such as an Assembly View) to change to reflect the variation, and apply mesh rendering where required – see Tools » Document Options for the Variant rendering settings.
Special strings, such as the VariantName and Variant Parameters can be placed in the drawing as free strings, or for a more universal solution, included in the title block of Draftsman sheet templates – see the Document Parameters dialog for a list of the available parameter strings.
When a saved Draftsman document is subsequently generated from an Altium Designer Output Job, the parameter special strings are interpreted in line with the Variant selected in the OutJob.
The Altium Draftsman PCB drawing capability is enabled in Altium Designer through the Draftsman software extension, which is automatically installed with Altium Designer – 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 Designer 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 the Altium Designer 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.
Contact our corporate or local offices directly.
Complete this form to request a free 15 day trial of Altium Designer: