Get email delivery of the Cadence blog featured here
You have placed components and routed the board. You are finally ready to send the design to a fabrication house to be manufactured. But wait, you have to perform a few tasks yet. You will start with backdrilling and then do the post-processing tasks - testpreps, thieving, NC drill, cross-section charts, artwork files, and generate reports. Let's get started with the tasks then.
Although surface-mount (SMT) is more common, our designs are still full of plated through holes and, of course, there are vias - blind, buried and what not. Now, if you have a high layer count PCB (printed circuit board) with thick backplanes with many through holes and vias, you will not want the unused portions or stubs that extend beyond the connected layer to distort high-speed digital signals that pass through them. So, your manufacturer backdrills (control depth drilling) to remove the stubs. But the pins and vias must be updated with the required data for them to be backdrilled.
You can easily verify and update pins and vias with the data required to perform backdrilling.
Use the Backdrill Setup and Analysis window (Manufacture – NC – Backdrill Setup and Analysis) to set up and verify backdrill information in your design. Specify the layer pairs – the two layers between which backdrilling is to be done, the objects to be backdrilled (pins, vias, or both pins and vias), any layers with connectivity that should not be cut along with the depth, and the number of possible backdrill locations (plunge). Also, set the parameters for padstacks that do not have backdrill data defined in the library or the design.
The Padstack Parameters tab of this window will inform you if padstacks do not have user-defined backdrill data. Just go ahead and use Pad Editor to define backdrill data for these padstacks. It's quite simple using the Secondary Drill, Design Layers, and Mask Layers tabs of Pad Editor. To bring up Pad Editor, choose Tools – Padstack – Modify Design Padstack, right-click a pad and choose Edit. You can verify the backdrill sizes from the Summary tab.
It is a good practice to view the log generated by Backdrill Setup and Analysis window to optimize backdrilling; for example, by removing, if possible, any layer pairs with say a single plunge. By the way, you can choose to either minimize electrical stub length or minimize layer pairs while analyzing and create layer pairs based on the result.
You might find the ability to display backdrill information on the canvas very useful. Just set Backdrill holes and Drill labels in in the Design tab of Design Parameter Editor (Setup – Design Parameters). You can also view a backdrill report (Tools – Quick Reports - Backdrill Report).
You will, of course, want your board to be tested to ensure your manufacturer can verify all is fine. Later on, you might want your service engineers to be able to troubleshoot the circuit easily. Well, for that you add test points - probe sites for test fixtures. PCB Editor gives you choices - create test points automatically or do that manually. You can then edit the test points individually to modify them. Just choose Manufacture – TestPrep and you have all your options.
Now is the time to add the spots (copper dots) on the board. You will uniformly distribute copper on the outer layers. Why? Because during manufacturing, you want the plating to happen uniformly. So, you 'steal' current from the areas that have less copper than say where you have a BGA. Go ahead, then, choose Manufacture – Thieving and update the Options pane.
PCB Editor adds 'thieves' as a group of vias. So, it is easy to perform any operation on them, say moving or deleting.
NC (Numeric Controlled) drill files will be used by your manufacturer to do exactly that - drill holes on the board. You will definitely want to verify all is well with the drill data in your design. You will also want to generate NC drill legend tables that appear on a fabrication drawing quantifying the number, type, and tolerance of plated and non-plated holes. Choose Manufacture – NC to see all the available options.
To create the legend tables, choose Drill Legend. To modify or verify NC drill data, choose Drill Customization.
Now is the time to speak Fab - get your design information in a format that will be understood by the manufacturing houses. Gerbers, of course, but not only that - as usual, PCB Editor gives you options beyond the traditional. So, choose Manufacture – Artwork and set the option you want. For example, you might want to set RS274X to generate just one file per layer.
Specify the layers for which you want to create artwork in the Film Control tab. PCB Editor will add film control for each etch subclass in the design, by default. But if the layout stackup does not match the artwork statckup, you will know because the Create Missing Films button will be active. You can always create the missing films for non-etch layers, say for the top or bottom silkscreen.
By the way, you might want to explore IPC-2581, which is an open global standard to communicate build intent to manufacturers.
The final task you will want to perform is, of course, to generate reports to verify different aspects of the board. Just choose Tools – Reports and then select the reports you want to generate, say Design Rules Check (DRC) Report and Summary Drawing Report.
Click Generate Reports and you are done!
After the tedious tasks of managing constraints and routing, the final tasks to prepare your board for manufacturing seem easy. But this phase require alertness and keen eyes to avoid manufacturing issues. Of course, the reports and verifications built into the PCB Editor environment help you avoid most of the possible issues. We have touched upon almost all the post-processing tasks and mentioned how PCB Editor can be of assistance in these tasks. But if you want to try out these tasks with a real design or learn more about IPC 2581 or cross-section charts, check the Rapid Action Kit (RAK) on Backdrill, Post Processing, and Report Generation, available on Cadence Online Support.