Draftsman Enhancements (New Feature Summary)

Altium Designer’s Draftsman® feature offers an advanced new way to create graphical documents for board design production. Featuring a dedicated graphics editor with a rich set of drawing tools, Draftsman produces custom assembly and fabrication output documents that are able to accurately communicate manufacturing intent.

With the release of Altium Designer 17, the Draftsman documentation system includes a range of enhancements and additional features that add to its flexibility while improving drawing efficiency. These include new dimension options, additional drawing object properties, improved rendering performance, and more.

Ordinate Dimensions

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.

Ordinate Dimensions are relative to the first-placed point.

To place an Ordinate dimension object in Draftsman, select Ordinate Dimensions () from the main Place menu or the Dimensions dropdown menu (), or select that 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:

1. Hover the cursor over the drawing view until the desired point or object edge is highlighted.
2. Click to select this as the first (reference) point, then move the cursor and click to set the extension position and angle.
3. Continue selecting points to create the full series of Ordinate Dimensions.

The set of dimensions behave as one object, and can therefore be edited in the Properties panel or moved as a single entity. Note however that individual dimensions may be added or removed when the Ordinate Dimension object is selected.

A series of Ordinate Dimensions are treated as one object, but individual entries can be added and removed.

Dual Units

The Units for Draftsman objects, nominally set to Metric or Imperial, can be configured to show as both types on individual objects, or as a global setting. This provides an additional level of dimensional clarity and further protection against manufacturing conversion errors.

Dual Units can be enabled and configured on an individual dimension object basis in its respective Properties panel options. Select a placed dimension in the workspace, then check the Dual Units option in the panel's Units section. The type of unit (millimeters, mils, inches) is selectable for both the Primary and Dual Units, as is the unit Precision.

Dual Units are available for Draftsman objects that use active units, such as:

• Linear Dimensions
• Radial Dimensions
• Ordinate Dimensions
• Layer Stack Legend
• Drill Table
• Bill of Materials

Selectable Dual Units can also be configured for the active document (and therefore, ultimately, a Template) in the Document Options dialog under the Units tab. Open the options dialog with the Tools » Document Options menu command, the main toolbar icon (), or by selecting that command after right clicking in the drawing workspace.

Dual Units, and their respective precision settings, can be applied on a per document basis.

Assembly View Silk Screen

In some circumstances it may be desirable to including the board design's Silk Screen overlay in an Assembly drawing view – such as where an existing overlay includes important production information.

To enable the existing Silkscreen layer for a placed Assembly view, simply select the view and check the Show Silkscreen option in the Properties panel. The correct overlay (Top or Bottom) will be shown for the currently selected View setting.

Note that component graphics and designators on the Silkscreen layer are not displayed, as these elements are automatically handled by Draftsman. All other Silkscreen objects are displayed, including Special Strings. In the above example image, where the Silkscreen overlay has been enabled for an Assembly drawing, the special strings under the REVISION No and DOCUMENT ID labels have been converted to the current PCB project values.

Support for Back Drilling

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).

The Layer Stack Legend view showing backdrilling enabled between the Top and Signal 3 layers, and the Signal 4 and Bottom layers.

Note that the Back Drill Pairs are established in the Drill-Pair dialog in the PCB editor – opened from the button in the Layer Stack Manager dialog (Design » Layer Stack Manager).

Created Back Drill Pairs (marked with a 'BD' prefix) in the Layer Stack Manager Drill Pair dialog.

Multiple Fabrication Views in Templates

Draftsman offers a flexible approach to creating templates that can be applied to new documents. Document Templates define a Draftsman document's content, and support multipage documents, data for the main document attributes (tables and lists, drawing types, etc) and elements created by the drawing Editor that do not directly depend on the PCB's design content.

Along with other types of Drawing Views – such as Assembly, Drill Drawing and Layer Stack views – a template can include any number of Fabrication Views, which might be spread over several sheets.  Each Fabrication View would be assigned to a board layer, and its content determined by that layer in the current PCB design.

For convenience, a Document Template can be created using a simple (dummy) PCB design, since the design content will not be used when the template is applied to a new Draftsman document. A Fabrication style Template might normally include Drill Drawings, the Layer Stack and additional information, plus Fabrication Views for all available layers or a specific set of layers. These would typically be a set of Signal/Plane, Mask, Paste and Silkscreen layers (usually on individual document Sheets).

All Fabrication Layers

To create a Fabrication style Template that will include all possible Fabrication Layers from the active design, it is only necessary to place a single Fabrication View and then set its Layer (under View) to All (for document template) in the Properties panel.

A special All Layers view option, intended for Template creation purposes, is available for Fabrication Views

When saved as a Document Template (File » Save As) and subsequently applied to a new Draftsman document, the template’s ‘all layers’ setting instructs Draftsman to create Fabrication Views for all available Layers in the active design (at one per sheet). The included layers can be restricted to specific groups of layers (Silkscreen, Solder Mask, etc) using the Layers checkboxes available in the New Draftsman Document dialog.

The Fabrication Views included in a document that is based on a Template configured for 'all layers' are determined by the new document Layers settings.

Specific Fabrication Layers

To create a Template that will include Fabrication Views assigned to specific layers, simply place multiple Fabrication Drawings and assign each to the desired layer.  In the below simplified example, Fabrication Views have been added to a single drawing Sheet for a range of Signal Layers (only) – as indicated in the Layer Stack Legend view.

Draftsman Templates can be created from an existing design, or a purposefully simplified design (lacking PCB content) to make the task easier – this will also minimize the Template file size.

When the Draftsman document is saved as a Document Template (File » Save As – Altium Draftsman Document Template (*.DwfDot)) and that Template subsequently used for a new Draftsman document, the Template’s layout, including its Sheet properties and Drawing Views, are applied to the new document for the currently active PCB design.

Where any of the template’s constituent layers are not available in the current PCB design, the Fabrication View assigned to that Layer will default to the current design’s Top Layer.

When Draftsman applies a template with multiple Fabrication Views to the current design, any unmatched layers will default to the Top Layer view.

Custom Table

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.

Nominate the number of cells in the Table's rows and columns – these can be modified later via a cell's right-click Table commands.

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.

Configure the Table style to suit through the Properties dialog.

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.

The right-click Table commands offer a range of standard table manipulation functions.

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.

A Custom Table can be constructed to host a wide range of different PCB assembly and fabrication information.