Tutorial

This page covers designing a simple board with Razen. This includes:

  • Initial setup
  • Using parts from existing libraries
  • Creating a new part
  • Routing a board
  • Generating gerbers for fabrication

First Start

The first time you start Razen, you’ll have to configure a few options. The only required setting is a username. If you want to use a Mercurial server for sharing libraries or designs, you should use your credentials for that server here. Otherwise any username will suffice. This username will be used to tag your changes to any designs you make.

_images/tut01.png _images/tut02.png _images/tut03.png

Once configured choose ‘Start a new project’ and you’ll be presented with an empty project. Lets have a look around the Razen interface before you start your schematic.

Schematic 1

Make sure you’re in the schematic view and click the Part tool (shortcut ‘A’). This will bring up your parts library. A standard set of libraries is distributed with Razen, including the passives and a variety of other components.

_images/tut06.png _images/tut07.png _images/tut08.png

Select the r_0207-10 resistor from the “razen/lib-rcl” library and click “Add Part”.

_images/tut09.png _images/tut10.png

You will now have a resistor symbol following your mouse. You can click to place resistors in your design. Place two resistors, then press escape to leave the part tool and return to selection mode.

Now, if you select a resistor you will see its properties displayed on the right, and the tools appropriate to it on the left. Lets rotate and move the resistor. With it selected click the rotate tool (shortcut ‘R’) and the resistor will be rotated 90 degrees. Now enter the move tool (shortcut ‘G’, or double-clicking the part), move the resistor, then left-click to place it. Once they’re arranged to your liking, add and move a capacitor (c_0305-03).

_images/tut11.png _images/tut12.png _images/tut13.png

Now lets draw some wires between the resistors and capacitors. Choose the wire tool (shortcut ‘W’) and draw some wires connecting the 3 parts. The center of the square is the active part of the pins and once a wire is placed there it will stay connected even if you move the part.

If you switch to the layout view now, you will see the 3 footprints for your parts, as well as yellow airwires between the pins you connected in the schematic. These show which connections still need to be routed - you’ll do that in the layout section of the tutorial.

_images/tut14.png _images/tut15.png _images/tut16.png

Next you’ll want to add a 555 timer chip, but it doesn’t exist in the standard libraries. So lets make a new part. First make sure to save your project: click save and enter “tutorial” as the name of your project.

Creating Parts

Lets create a new 555 part. A part is made up of a symbol and a footprint (with a mapping between symbols pins and footprint pads). Parts can share symbols or footprints (like all resistors sharing a common symbol).

First click the “New Part” entry in the file menu, which will show the New Part dialog. First lets choose the library you’ll use for this part. Libraries are of the form <username>/<libraryname>, where the username is used when sharing the library via a Mercurial server. For now, lets create a new ‘tutorial’ library.

_images/tut17.png _images/tut18.png _images/tut19.png

Click the “New ...” button and enter “lib-tutorial” as the library name, and enter a description of the library if you wish. Click ok and the library will be created and shown with your username. Now enter the names for the part symbol and footprint. If this part was using a shared symbol or footprint (like the resistor example), you could select them using the “Use existing” buttons. For this part simply enter “ne555” as the symbol, and “dip8” as the footprint. This will automatically generate the part name “ne555_dip8”.

Click ok and a new part design will be created. The part design view is almost exactly like the project design view. The schematic view shows your part symbol, and the layout shows the footprint. The main difference from project views is that you have access to slightly different tools when editing parts - specifically the pin and pad tools.

Now you could draw your part symbol and footprint using the Line, Arc, Text, Pin and Pad tools, but since this is a relatively common part, we can use a script to auto-generate the basic outlines of your symbol and footprint.

_images/tut20.png _images/tut21.png _images/tut22.png

First, click the tools -> scripts -> dip generator menu. This will bring up an options dialog where you can change the pin count to 8. Click ok and a basic 8 pin dip symbol and footprint will be generated. Lets rename the pins to match those of the 555 as in the second screenshot above. To rename a pin, simply select it, right click, choose ‘rename’, then enter a new name. Once the pins are renamed, you can move and rotate them into the more common 555 layout.

Now that you have your symbol and footprint drawn, you need to map symbol pins to footprint pads. In simple parts no mapping is needed, as long as all pins have a pad with a matching name. In your 555 case, you need to explicitly map the pin to pad names. Click the tools -> pin mapping menu and the pin mapping dialog will appear.

_images/tut23.png _images/tut24.png _images/tut25.png

The pin mapping dialog shows pin names, pad names, and mappings between the two. Initially there will be no mappings, so select a pin and a pad, then click “Map”. This will remove the pin and pad from their respective lists and add a mapping. The pinout for the 555 is as follows:

Pin Pad
gnd 1
trig 2
out 3
reset 4
ctrl 5
thr 6
dis 7
vcc 8

With your symbol and footprints drawn and the pins mapped to pads, your 555 part is almost complete. The last thing you need to do is set a part prefix. This is the character(s) used to prefix part names in designs (like ‘R1’, or ‘C42’).

_images/tut26.png

Deselect anything you have selected in the main view (press Escape) and the part properties will be visible in the properties panel. Change the ‘prefix’ property to ‘U’.

Your part is now complete. Save the part and switch back to your tutorial project.

Schematic 2

Back in the project, you can now add the 555 timer part to the schematic. Click the part tool, select the “ne555_dip8” part and place it on your schematic.

_images/tut27.png _images/tut28.png

Once the 555 is placed you can continue adding wires to your schematic using the Wire tool. Finish the schematic by adding another resistor and LED (from the razen/lib-led library) to the output pin of the 555, as well as a 2x1 header for power (library razen/lib-conn-header).

_images/tut29.png _images/tut30.png

With all the parts and wires in place, you can finalise the design by renaming the parts appropriately and setting part values where appropriate (using ‘value’ property in the properties panel).

Your schematic should now be complete. Make sure to save it before starting on the layout.

Layout

Switch to the layout view by clicking the view name in the bottom left of the design view. You will see the footprints for all the parts you added in the schematic, as well as yellow airwires indicating traces that still need to be routed. The airwires are automatically generated from wires you place in your schematic.

_images/tut31.png _images/tut32.png _images/tut33.png

First you’ll want to reorganise your parts on the board. Hide the airwires by double-clicking the Airwire layer in the layers panel. Once hidden you can move the part footprints around to a more appropriate layout. As with the schematic, this is done with the Move (G) and Rotate (R) tools.

_images/tut34.png _images/tut35.png

Once you’ve reorganised the footprints, you can draw a board border using the Line tool. Now, un-hide the Airwire layer (double-click again), and you can start routing traces.

_images/tut36.png _images/tut37.png _images/tut38.png

To route a trace, select an airwire you wish to route and enter the Route tool (E). You will now be laying the traces for that airwire. The nearest pad to your cursor will be indicated, showing you were to route. Left-click to place traces and once you complete the trace, you will automatically be returned to select mode (and the airwire will disappear, indicating it is correctly routed).

_images/tut39.png _images/tut40.png _images/tut41.png

Continue routing all the remaining airwires using the Route tool. You can change trace thickness, layer, and routing style with the tool options on the left while in the Route tool.

Once all airwires are routed, your board is almost complete. Add a few mounting holes in the corners of the PCB using the Drill tool (modifying the drill diameter to an appropriate value).

_images/tut42.png _images/tut43.png _images/tut44.png

Some of the part names will probably overlap pads, so you should probably move them to more visible positions. Select a part and click the Splitname tool. The part name will now be moved to a separate object which you can now move and rotate as needed.

Finally, you can also add some extra labels to the board using the Text tool (Click the text tool then type the text in the command prompt, followed by enter).

Gerbers

To manufacture our board we’ll need gerber files. To generate gerbers, simply click the file -> export -> gerber menu. Your layout will be exported to gerber files in the project directory. A zip file will also be created containing all the gerbers, ready to be sent off to manufacturing.

_images/tut45.png