Creating the Fabrication Drawing in Draftsman
In previous chapters, you have learned how to fully create the schematic diagram, the PCB, how to upload files for manufacturing, and how to create your own components for libraries. The next step is to add drawings to fully document the created device. The Draftsman extension (included in Altium Designer by default) is used to create and edit drawings. This extension is tightly integrated with Altium Designer and allows you to create, edit, and update any drawings of your device seamlessly. If any changes are made in the PCB design, the entire drawing can be updated with a few mouse clicks. In this chapter, we will create a fabrication drawing for our PCB.
First, we need to add a Draftsman document to the project structure.
Make sure that the Kame_FMU project is open and active. Right-click on the project name in the Projects panel then select Add New to Project > Draftsman Document.
In the New Document dialog that opens, choose from one of the document templates that are in your workspace. You can create a separate template for the document so that you can generate the required drawings of a particular type in just a few mouse clicks. For now, select [Default]; our drawing will be created manually. Make sure that Kame_FMU is selected in the Project (PrjPCB) and Document (PcbDoc) drop-down menus and all layers are enabled in the Layers region. Click OK to create a document. A new Draftsman document will open in the design space and the new Draftsman document (PCBDwf) has been added to the project in the Projects panel.
The sheet format must first be specified in order to place all the necessary PCB information on the document. We already know in advance that all the information we need will fit on the A3 sheet, so we will choose that sheet template.
Open the Properties panel using the Panels button at the lower-right of the design space then open the Page Options tab. In the Formatting and Size region, enable the Template option to select a document sheet template from a pre-created template. In the Template drop-down, select Top Sheet ISO-A3 (v.3) from the Draftsman Templates region. (Please note that this region includes all cloud-based document templates as well as local pre-installed document templates. You can change the default template storage folder on the Data Management - Templates page of the Preferences dialog.) The sheet in your design space will change to that template.
Tip: In addition to cloud and local sheet templates, you can use one of the default sheet sizes (such as A4, A3, etc.,) by selecting the Standard option on the Page Options tab in the Formatting and Size region of the Properties panel. If you wish to use a sheet of a different format, you can specify its dimensions manually by selecting the Custom option. You also can change these sheet parameters anytime as the drawing is being created.
We can now begin placing the necessary objects on the drawing. Let's start with the most important thing in the fabrication drawing - layered views of the printed circuit board.
Select Place > Board Fabrication View from the main menus. The top layer of the PCB will be attached to the cursor; click to place it.
It is difficult to see any small details at this scale, so let’s increase the scale to 2:1. Double-click the placed Board Fabrication View. In the Scale region of the Properties panel, you can choose either one of the standard scales in the drop-down or enable Use Custom Scale to enter your own. Select 2:1 from the Scale drop-down menu to enlarge the view. The scale will also be updated in the view description on the design space. Place the view as shown in the figure below.
Now we need to place the views of the other layers. You can place them as described in step 4, each time selecting the desired layer and scale in the Properties panel. However, we will do this in a slightly different manner. We will set up and copy the current layer view then configure the layer we need for each view. Draftsman automatically selects the colors of the layers based on their color on the board. Let’s make the current and all future layers to display monochromatically.
Select the placed Board Fabrication View. Open the Layers tab of the Properties panel to access layer settings. Click on the colored square to the left of the Top, GND2, L3, L4, GND5, and Bottom layers then select black as the color for each as shown in the images below.
Click on the Board Fabrication View to select it then press Ctrl+C to copy the view.
Press Ctrl+V to paste the view then, using the image below as a reference for positioning, copy and paste additional views and as shown in the figure below. Pay attention to the guidelines while placing to place the views in a plain array. After pasting, your Draftsman document should look like the figure below. In th next steps, we will configure these layers as Top, GND2, L3 layers on the upper side, and L4, GND5, and Bottom layers on the bottom side.
Select the upper-middle view. We will define this layer as the GND2 layer. Open the General tab of the Properties panel. In the Properties region, select GND2 from the Layer drop-down menu. Once selected, the view and its name will be updated and display the as GND2 layer.
Using the same approach, select the upper-right view and define its layer as L3.
Using the same approach, define its layer as L4 for the lower-left view, GND5 for the lower middle view, and Bottom for the lower-right view.
Let's set the opposite side of the view for the lower row of views. This raises the drawing readability considerably because when we flip the physical board, we'll see that the current layers are mirrored. Using right-to-left selection, select the lower row of views. In the Properties section of the Properties panel, use the View Side drop-down to choose Bottom.
Next, we will add a Layer Stack Legend to fully describe the PCB layers configuration.
Select Place > Layer Stack Legend from the main menus. Place the legend under the placed views. If the inserted legend overlaps some of the views, we will correct it in the next step.
Click anywhere in the legend to select it. In the Properties region of the Properties panel, in the Display Mode drop-down, select Align Table Rows or Default
Adjust the Layer Stack Legend position. It should be placed under the views and should not overlap them.
Now let's add and configure a Drill Drawing View and Drill Table to our document.
Select Place > Additional Views > Drill Drawing View from the main menus and place the view to the right of the PCB layer views as shown in the figure below. Select the placed view and set its scale to 2:1 in the Properties panel.
In the Drill Drawing View, the drill symbols overlap each other, so we need to adjust their size. Select the placed Drill Drawing View then click the Drill Symbols button in the Properties region of the Properties panel. The Drill Symbol Configuration dialog that opens lists all the holes that are present in the design with their parameters and corresponding symbols. Each hole is in a separate row. Select a row/hole to view the properties of that hole in the lower region of the dialog.
Tip: You can choose a custom symbol for any hole by using the Symbol Graphics drop-down in the dialog.
In the HoleSize column, find and select the 2.50mm hole. In the lower region of the dialog, set its Symbol Size to 3.0mm.
Using the same approach, set the 0.60mm hole to Symbol Size 1.5mm, and the 0.20mm hole to Symbol Size 1mm. Click OK to save the changes and close the dialog. The Drill Drawing View should now look like the figure below.
Now let’s place a Drill Table that lists all the used holes. Select Place > Drill Table from the main menus and place the table under the Drill Drawing View. When the table is selected, you can manage its columns on the Columns tab of the Properties panel. Make only the Symbol, Count, Hole Size, and Plated columns visible. The Drill Table should look the same as in the figure below.
Next, we will add a Transmission Line Table to the drawing. This table is placed and configured similarly to the Drill Table.
Select Place > Transmission Line Table from the main menus. Place the table under the Drill Table.
As you can see, the table does not fit the width of our drawing. Let's reduce the font size and turn off columns we do not need.
Select the placed Transmission Line Table. On the Columns tab of the Properties panel, disable the visibility of the Narrow Trace Width, Gap, Reference layers, and Substack columns. In the Rows region, disable the visibility for the 2 and 5 Impedance Ids. These are reference layers and there are no tracks placed on these layers.
On the General tab of the Properties panel, in the Properties region, uncheck Use Document Font for Caption Font and Rows Font. Set the font to Arial and the font size to 12 font for both. Your Transmission Line Table should look as shown in Fig. 24.
Now, for the final touch, we need to add the description text to our drawing.
Select Place > Annotations > Note from the main menus. Place the note between the Transmission Line Table and the main drawing description that displays data. such as the engineer, designer, checker, etc.
The Note contains default values so it needs to be edited line by line. In the Selected Element region of the Properties panel, you can set up string parameters, change their order, add new rows, and delete unnecessary ones. Select the second line of the note in the design space then click to delete it. Now delete the remaining second line.
While string number 1 is selected, select None from the Border drop-down menu.
Enter “FINISH: ENIG PER IPC-4552” in the Note Description field. Click the Add button to add a new string.
Enter “ALL HOLES FINISHED SIZE AS SHOWN” text in the Note Description field.
Now your fabrication drawing is ready. As a result, your drawing should look like the one shown in the figure below. All we need to do is save this document and upload it to the server.
Tip: You can add as many sheets to the drawing as you want! To add a sheet to a document, right-click in any blank space in the drawing then select Add New Sheet. A new sheet will appear at the bottom of the current sheet.
Select File > Save from the main menus then save the document name as “Kame_FMU_Fabrication”.
Right-click on the project name in the Projects panel then select Save to Server. Enable the Kame_FMU_Fabrication.PCBDwf file for commit if it is not enabled. Enter “Fabrication drawing has been added” in the Comment field then click Commit And Push to make this document available online.
Tip: If your PCB layout has been changed after creating the drawing, no problem. You will not have to redo the drawing. Choose Tools > Import Changes from <PCB name>