Main page: Streamlining Board Design Documentation with Draftsman
Altium Designer's Draftsman editor provides tools for creating multi-sheet fabrication and assembly drawings in an automated manner based on the project's PCB document.
Adding and Configuring the Draftsman Document
Main page: Setting Up a Draftsman Document
To start creating a new drawing, you need to add a new Draftsman document to the project. Since a Draftsman document is a source document of the PCB project, the process is very similar to adding documents of other types, like schematics or PCBs.
Adding and Configuring a New Draftsman Document
-
Right-click the project entry in the Projects panel and select the Add New to Project » Draftsman Document command from the context menu.
-
The New Document dialog will open. Select the [Default] entry in the Templates list and make sure that the correct project and PCB document (Multivibrator.PrjPcb and Multivibrator.PcbDoc) are selected in the Project and Document drop-downs.
-
Click OK in the dialog. A new blank Draftsman document will open.
-
Right-click on the Draftsman document entry in the Projects panel to select the Save As command and name it
Multivibrator.
-
If the Properties panel is not visible, click the Panels button at the bottom right of the design space and select Properties from the menu that opens.
-
When no object is selected in the document, the Properties panel presents the document options. On the Page Options tab of the panel, select Template in the Formatting and Size region, then select the ANSI B Landscape Draftsman template under the section of your Workspace in the Template drop-down.
Adding Drawing Views
Main page: Working with Views
Draftsman allows a range of automated production drawings to be placed directly onto a Draftsman drawing document. The drawing data are extracted directly from the source PCB document.
When the PCB data has changed, you can refresh the data in Draftsman by selecting the Tools » Import Changes From <PCBDocumentName>.PcbDoc command from the main menus.
Adding Drawing Views
-
Place an assembly view:
-
Select the Place » Board Assembly View command from the main menus.
-
A top-side assembly view will be attached to the cursor. Hover the cursor so the view appears in the top left part of the drawing and click to place it.
-
Double-click the placed assembly view to open its properties in the Properties panel. On the General tab of the panel:
-
Select the
2:1 scale value from the Scale drop-down in the Scale region.
-
Select the
Silkscreen option from the Designator drop-down in the Component Display Properties region.
When the Silkscreen option is selected, the position of component designators on the assembly view will be defined by the positions of corresponding designators on the overlay layer in the PCB document. The position of designators can also be graphically modified by using the Ctrl+Click, Hold&Drag shortcut. Use the Spacebar to rotate a selected designator through 90° increments.
-
Place fabrication views:
-
Select the Place » Board Fabrication View command from the main menus.
-
A top-layer fabrication view will be attached to the cursor. Hover the cursor so the view appears at the right of the placed assembly view and click to place it.
-
Double-click the placed fabrication view to open its properties in the Properties panel. On the General tab of the panel, select the
2:1 scale value from the Scale drop-down in the Scale region.
-
Place another fabrication view to show the bottom layer. Select the Place » Board Fabrication View command from the main menus.
-
Hover the cursor so the view appears at the right of the placed fabrication view and click to place it.
-
Double-click the placed fabrication view to open its properties in the Properties panel. On the General tab of the panel:
-
Select the
2:1 scale value from the Scale drop-down in the Scale region.
-
Select the
Bottom Layer option from the Layer drop-down in the Properties region.
-
Place an isometric view:
-
Select the Place » Additional Views » Board Isometric View command from the main menus.
-
Hover the cursor so the view appears at the right of the placed fabrication views and click to place it.
-
Double-click the placed isometric view to open its properties in the Properties panel. On the General tab of the panel:
-
Select the
2:1 scale value from the Scale drop-down in the Scale region.
-
Select the
Front option from the Face side drop-down in the Properties region.
-
Place a layer stack legend:
-
Select the Place » Layer Stack Legend command from the main menus.
-
Hover the cursor so the layer stack legend appears below the placed fabrication and isometric views and click to place it.
Annotating the Drawing
Main pages: Drawing Annotation, Dimensioning & Tolerances, Working with Tables
To add important information to a Draftsman drawing document, a number of annotation, dimensioning and other tools are supported.
-
Object dimension graphics can be placed on board views (including assembly and fabrication views) to indicate the lengths, sizes, and angles of the object outlines or the distance between nominated objects.
-
Industry-standard geometric dimensioning and geometric tolerances symbolic elements that define the manufacturing properties of objects included in a drawing are supported.
-
Tables of different types can be placed to provide a simple, visual way to convey crucial information for the PCB fabrication and assembly processes.
-
A range of graphical element tools that can be used to place basic, free-form drawing elements in a document is also provided.
Annotating the Drawing
-
Place linear dimensions for the horizontal and vertical size of the board:
-
Select the Place » Linear Dimension command from the main menus.
-
To place the dimension's first reference point, hover the cursor over the top edge of the PCB on the assembly view and click when the edge is highlighted orange.
-
To place the dimension's second reference point, hover the cursor over the bottom edge and click when the edge is highlighted orange.
-
Move the cursor at the left of the view and click to set the position of the dimension text and its associated extension lines.
-
You will stay in dimension placement mode. Similarly, place another dimension by sequentially clicking the left and right edges of the PCB on the assembly view and clicking below the view.
-
Right-click to exit dimension placement.
-
Place a BOM table:
-
Select the Place » Bill Of Materials command from the main menus.
-
Hover the cursor so the table appears below the assembly view and click to place it.
-
Place callouts displaying the BOM positions of the components on the board assembly view:
-
Select the Place » Annotations » Callout command from the main menus.
-
Hover the cursor over the edge of the
Q1 transistor projection on the board assembly view so it is highlighted and click to place the callout pointer.
-
Move the cursor at the right of the view and click to confirm the placement of the callout source text.
-
Identify one more source for the same callout by hovering the cursor over the edge of the
Q2 transistor projection and clicking.
-
Right-click to complete the placement of this callout. You remain in callout placement mode.
-
Place callouts for other components on the view as shown in the image below.
-
When all required callouts are placed, right-click to exit callout placement.
-
Save the project to the Workspace.
