Creating the Assembly Drawing in Draftsman
In the previous chapter, we created the drawing needed to fabricate a PCB specifically as a component of a future unit, so we need the assembly drawing to correctly place all components on the PCB. In this chapter, we will create an assembly drawing that is required to assemble a PCB with the components for the final working device. It is recommended to create the assembly drawing separately from the fabrication drawing, so let’s create a new document in the project.
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, select [Default] as the template. We will not use a pre-installed template. Make sure that Kame_FMU is selected in the Project (PrjPCB) and Document (PcbDoc) drop-down menus and all layers are activated in the Layers region. Click OK to create a new 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.
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 size of this template will be more than enough to fit all required views with the PCB dimensions. 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.
Now let's add the views of our PCB:
Select Place > Board Assembly View from the main menus. Place the view at the upper left corner of the sheet as shown below.
It is difficult to see small details at this scale, so let’s increase the scale to 4:1 so it will be easier to place component designators and considerably increase the readability of the printed drawing.
Select the placed Board Assembly View. In the Scale drop-down of the Properties panel, select 4:1. If the view has shifted after scale change, move it so that it completely fits on the sheet.
The view is not suitable for use because designators are placed inside the component body, and there are rectangles instead of mounting holes. Let’s fix these.
Click on the PTH1 rectangle to select it.
In the Component Display Properties region of the Properties panel, enable the Apply changes to all instances of same BOM item option. This option is useful for changing the properties of the all same components at once.
Now let’s change the component body display type. In the Component Body drop-down, select Assembly drawing type, The components will change as shown in the figure below.
Why didn't the mounting hole initially show up like this? If we look at other components, we will see the same Default display for them as for our mounting holes, but their display quality is much better. The answer lies in the logic of this tool. While generating the Board Assembly View, the projection of a board component's 3D model is used by default, but if a 3D model of a component is not available, Draftsman tries to get the information based on the silkscreen of this component. In our case, the mounting holes didn’t have a 3D model or silkscreen graphics, so Draftsman drew them as a Bounding Box based on the component size. This is how the different component body display types look.
Tip: You can set the Component Body display type for all the components on the PCB - just click on the empty place on the PCB and apply the desired type.
Now let's add a side view and a bottom view.
Select the view then press Ctrl+C to copy it. Select the lower-left corner as a reference point.
Press the Ctrl+V key combination to paste the copied view then copy another and past in the locations as shown in the figure below.
Tip: You can place the new views by using Place > Board Assembly View, but you will need to specify the Scale value each time after placement.
Select the middle view. In the Properties region of the Properties panel, use the View Side drop-down then select Left. Move the Left view if it was shifted and place it in line with the other views as shown in the figure below.
Now select the right view. In the Properties region of the Properties panel, use the View Side drop-down then select Bottom. Move this view if it was shifted and place it in line with the other views as shown in the figure below.
The next important step is to place all the designators so that they can be read and it is evident that they belong to a certain component. Designators can be moved individually, for the entire board, or for a set of identical components.
Select one of the three capacitors above the U12 component on the top side view.
In the Component Display Properties region of the Properties panel, enable Apply changes to all instances of same BOM items.
Open the Designator drop-down menu then select Right. The designators of the selected component and the same component instances will be moved to the right side. Select the other component from this row and apply the same position from the Designator drop-down. You can quickly set the correct position for a large number of repetitive components, which can save you a lot of your time.
Tip: If you want to set the same Designator position for all components, select the view then change the Designator to the desired type in the drop-down menu in the Component Display Properties region of the Properties panel.
You also can manually move the designators. Select the U3 component designator at the upper-right corner of the top view.
Press and hold the Ctrl key then drag it to the top of the component. While moving the designator, there is a red reference line that shows it belongs to that specific component. This feature can help you unravel situations with high placement density when designators are placed very close to each other. Release the mouse button to fix the designator placement as shown in the figure below. While the designator is selected, you can change its size by specifying the desired value in the Designator Font Size field of the Component Display Properties in the Properties panel.
Tip: Do not release the Ctrl key while moving designators.
Tip: You can rotate the designator while moving it by pressing the Spacebar. It’s not good practice to rotate designators if it is not required since a designator placed in the same direction as a component is much easier to read.
Using the methods described above, place designators so that they are all visible, readable, and it is evident that they belong to a particular component. You can use the figure below as the guideline for the designators’ placement.
You could use this drawing for your PCB, however, the drawing is not completed yet. We’ll add the basic dimensions of the PCB. First, let’s specify linear dimensions. Before starting, ensure that all Snapping options are enabled in the General region on the General tab of the Document Options mode of the Properties panel.
Choose Place > Linear Dimension from the main menus or from the Active Bar.
Hover your mouse over the left border on the Top side view to begin placement of the dimension. The suggested dimension point or line will change to orange. Click on the left border to select it as the starting dimension point.
If you selected the line primitive, a dimension of the selected side will be attached to the mouse cursor. Click on the right border of the view to set this side as the second dimension point.
The last step is to place the dimension. Place it above the view as shown in the figure below.
Using the same approach, place a linear dimension for the left side as shown in the figure below.
We also need to place the size of our mounting holes. Move the cursor to the lower right corner of the Top side view. Select Place > Diametral Dimension from the main menus or from the Active Bar.
Place the Diametral Dimension for this hole as shown in the figure below. Right-click to exit placement mode.
Select the placed dimension. Since we have two of these mounting holes, we can specify that in the footnote. In the Diametral Dimension mode of the Properties panel, in the Value region, enter “ x2” in the Suffix field to display the text after the diametral dimension.
Now let’s place a center mark for our mounting holes.
Choose Place > Annotation > Center Mark from the main menus or select it from the Active Bar. The Center Mark object will be attached to the cursor.
Hover the mouse over the upper left mounting hole on the Top side view. When the Center Mark snaps to the center of the hole, click to place it. Your result of this step should look as shown in the figure below.
Place the Center Mark for all remaining mounting holes on the Top and Bottom side views.
Add the remaining dimensions as shown in the figure below.
Now let's display our board in an isometric form.
Select Place > Additional Views > Board Isometric View from the main menus then place the Board Isometric View under the Top side view.
Select the view then set its Scale in the Board Isometric View mode of the Properties panel to 4:1. Set the Location in the Title region to Center-Above and Face side in the Properties region to Front. Move the location of the Board Isometric View as shown below.
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 the File > Save from the main menus then save the document name as “Assembly”.
Right-click on the project name in the Projects panel then select Save to Server. Enable the Kame_FMU_Assembly.PCBDwf file for commit if it is not enabled. Enter “Assembly 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>.PcbDoc from the main menus to update all graphics on the drawing to the actual state.