OK, further to Part 1 of this blog where we created a schematic, now it’s time to move to the PCB.
If you still don't have your license, get a trial from here:
And some more information from here:
Open up the project (well, if it’s not open already..) and click on “Project” → “Add new PCB”. This generates a blank PCB document with a default file name. Go ahead and give it a name. I like to keep it coherent with my schematic file name, so I’m going to name this “LED_Flasher_PCB”.
The next thing to do is to set the Grid size and units on the far right of the ribbon. The default uses Imperial system of measurement, I’m going to use the Metric and set snap grid size to 5mm. Also note, it helps to set the Origin to the (0, 0) if that is not the default origin already. This might be a little tricky to move the mouse to the exact position, but should come with a little practice. Once you set the Origin, click on “Absolute Origin” to move the origin of the board.
Now type 5mm into the Snap Grid box and hit return. Your blank PCB document should change as follows:
The next thing to do is to set the board shape. Navigate to Board → Edit Board Shape and your blank PCB should now be editable for shape as shown below.
Go ahead and make the PCB’s shape as you like, but for the purposes of this blog, I’ll keep it at the default shape. You can see in the screenshot below that I’ve gone ahead to create a star shape. But, I’ll reset it back to the default to proceed further. When you are done, hit Save.
Now, it’s time to import the schematics into the PCB. Navigate to Project → Update Schematics in LED_Flasher, this brings up a dialog box showing the recent changes (if any). If there are any last minute changes in the schematic, you can cross check them here before starting to create the PCB. Once you are happy with the changes, click on “Close” to close the window showing you the changes.
Time to import the schematic into the PCB. Navigate to Project →Import changes to bring the components into the PCB. You will see an “Engineering Change Order” generated. This is how Circuit Studio handles changes between schematic and PCB.
Click on “Validate Changes” to check for any errors and once it’s done, you should have green ticks under the Status column to indicate validity of execution of all the changes. Then click on “Execute Changes” to execute the changes (duh!!). Anyways, once that is done, you should have your components imported into the PCB as shown below.
Drag these one by one into the PCB document and feel free to place them as you like. Once you are done, hit Save.
You can also view the configuration of your board by clicking on the Layer Select (LS) at the bottom of the editor window. A configuration window opens up giving you the options to change layer colours, silkscreen layers, signal layers etc.
Navigate to the “View Options” tab here and make sure theNet Names on Tracks Display is set to “Single and Centered” and also the “Show Pads Nets” options is ticked. Click on “Apply” then “OK”.
You can also change the grid size at this point depending on the placement you need. This is done from the Properties button under the Grids and Units group. I’ve set mine to step 1mm in X and a multiplier of 5x Grid as shown below. Click on “Apply” then “OK”.
It’s now time to set some design rules. You can view/modify the design rules for the current project from the Design Rules button under the Design Rules group in the ribbon menu as shown below. The defaults are 0.254mm for the tracks. I’m going to change them to 0.25mm.
Now, we’ll create a new rule for Width of the tracks on the net labels we specified in our schematic. These are the 9V and the GND nets. Right click on the Width and select new rule from the context menu. A new rule Width_1 is created with similar parameters as Width. Go ahead and change the name to 9V and select Net in the radio buttons. You will see that the drop down menu is now enabled and select 9V from the drop down. Do the exact same thing for the GND net as well, except select the GND net from the drop down and name the rule as GND. A screenshot for this is below:
I’ll also change the design rule for electrical clearance to be at 0.25mm instead of the default of 0.254mm.
TIP: Instead of changing every single value, you can change the 1 single value next to the drawing shown and hit return to change all the values in the table. The screenshot below shows the value changed next to the drawing but I have not hit return yet.
I’m also going to change the routing vias’ diameter to 1mm and hole size to 0.6mm similar to the above.
Now, let’s apply the rules we just defined. Click on the small arrow next to “Design Rule Check” under the Design Rules group in the ribbon menu. Then click on “Reset Error markers”. Right click on the project name under project explorer and save your progress.
It’s time to auto-route. You can also do this manually defining all the track angles, clearances etc, but for the purpose and scope of this blog, to keep it quick, I’ll use the auto-router. Go to the “Tools” menu and click on “Autoroute” and then select “All..”. The “Situs Routing Strategies” window should show up as below. Click “Route All” at the bottom of this window. The routing should start and within a few minutes completed with a message box showing the status. This is shown in the screenshot below.
At this stage, if you are happy with the autorouting, then great. If not, you can go ahead and make any changes you like and save the project when you are done. Double clicking on a track brings up it’s properties and you can edit them here. You can also change the design rules and auto route again. Double clicking on a component brings up it’s properties which can also be edited. Feel free to play around with the various options here and work your way through your design.
When you are happy, move on to Part 3 of this blog where I’ll show you how to run Design Rule Check, fix any errors, view the board in 3D, generate the output files to print the board and generate the BOM.
Don't forget to check Part 3..