...

Now that you have completed placement, you can adjust the shape of the board to fit your components. Press “1” to enter the board outline edit mode, and go to Design → Edit Board Shape. You can then drag the edges to conform to your component placement. Remember that the origin should still be the bottom left corner of the board, so I suggest moving your components to there and shrinking the top and right edges. Board dimensions should be in full mm!

...

In the bottom of the screen, you’ll see a bunch of tabs for all of the drawing layers in the design. Click on the Keep-Out Layer, and here you can draw the shape of your board using lines and arcs. Board dimensions should be in full mm, so set your grid accordingly!

Once you have a closed outline, press Shift + K to isolate only elements on the Keep-Out Layer. Window over all elements to select them, and convert that to your board shape using Design → Board Shape → Define Board Shape from Selected Objects.

...

Routing

Ideally during the placement process, you’ve started to form an idea of how you’d route things and placed your components in such a way to make this process as easy as possible!

Traces

To draw a trace, press Ctrl + W. If you move your mouse to the centre of a pad, you’ll see it snap in place when there is a green cross and a circle. Drag your mouse to draw out the trace, click anywhere to create a vertex, and click again or click on the centre of a pad to end the trace.

Some general rules of thumb:

• 0.25mm trace thickness unless you require otherwise

• Avoid acute angles

Route all traces except for ground, we will make those connections later!

Vias

Sometimes you may find that traces need to cross over each other. If this is the case, you can connect traces on different layers using a hole plated with copper, called a via.

We have a 2 layer board, which means signals can cross past each other on opposite layers. In my routing, I have used a via to allow the 12V trace to cross below some other components on the bottom layer (blue).

...

Polygon Pours

Now that all connections except ground have been made, we will connect all the grounds together by filling all remaining empty space on the board with a ground plane.

Use the Place Polygon Plane option in the top bar, and define the 4 corners of your polygon. Note that you don’t need to make the polygon definition the same shape as your board. You can use a rectangular polygon to cover a board with rounded corners, the copper won’t be poured where there is no board.

Cover both the top and bottom layers with a polygon, and assign the net to gnd in the properties panel, You should see that all ground pads are now connecting to the place through small tabs.

It’s also good practice to place a gnd via next to every gnd pad. While they might all be connected through the top side copper, the pour has to snake it’s way around all the traces and components. Having gnd vias ensures a direct connection through the bottom layer.

Silkscreen

The silkscreen comprises everything that will be printed on the exterior of the boards for labelling, etc. These are the Top and Bottom Overlay layers. If you click on the top overlay layer, you can more easily select and rearrange the component designators.

While on this layer, you can also add labels for the connectors as well as the board name and Midsun logo.

To add the logo, you can use Place → Graphics and draw out the area where you want the image to go, then selecting the file.

Design Rule Checks

For major rule violations, often the program will alert you in the form of green circles with crosses. However, this is not always the case. Near the end of your design, go to Tools → Design Rule Check → Run Design Rule Check, and address any issues in the report. Note that you can click on the hyperlinks to cross-probe to the affected area!

If you have no warnings or violations, get a lead to look over your board, you might be done!

...