We will now route the board using both sides like many commercial PCBs. Having said that, use a single side wherever possible if your PCB is made using an old-fashioned process. Many problems occur with double-sided PCBs, mostly from badly placed vias, as I’ll now explain. Figure 19 shows a cross-section of a double-sided PCB. Commercially produced PCBs have plated-through holes (PTHs), which means that the copper plating extends through the holes and joins the pads on the two sides of the board. A free via is a hole that is used purely to move a track from one side of the board to the other, rather than to mount a component. The plating carries current between the layers. Simple, manual processes cannot plate through holes, in which vias need more effort: A wire must be pushed through each hole and soldered top and bottom to join the layers of etch. The wires of through-hole components can also be used as vias. This works well for some components, such as resistors and capacitors. However, it fails for others, such as connectors, because it is impossible to solder the pad on top of the board – it is hidden under the base of the connector. The pins of an integrated circuit can be used as vias if they are soldered directly to the board but it is safer to put ICs in sockets for PCBs that are assembled by hand and these hide the pads too. Vias must therefore be placed with great care if the PCB does not have plated-through holes.To illustrate these problems, figure 20 shows the two-sided layout of the instrumentation amplifier as it might come from the autorouter. (I should admit that I fiddled the layout to make it worse!) It obeys the design rules but is hard or impossible to assemble by hand. • Several pins of resistors act as vias – R3 has two, for instance. These are easy. The general rule is to avoid vias wherever possible if your manufacturing process does not plate through holes. Every via requires two soldered joints (top and bottom), which dramatically reduces reliability. Now route your board for the instrumentation amplifier using both sides. 1. Re-open the unrouted version of your board. Fixup. Choose Setup > Constraints > Physical. . . from the menu bar and select the upper All Layers spreadsheet under Physical Constraint Set. This resembles figure 13 but has only a DEFAULT row. The column headed Vias probably shows VIA:VIA26. Click in this cell to open the Edit Via List. Remove VIA from the Via list on the right and click OK. The cell now contains only VIA26, which is what we want. Close the Constraint Manager and return to PCB Editor. 3. The new board wizard set up several spacings based on the minimum line width of 25 mils. Unfortunately it does not set up the spacing around vias, which is only 5 mils by default. This is too small for reliable construction by hand and should be increased to match the other spacings. Fixup. Choose Setup > Constraints > Spacing. . . from the menu bar to open the Constraint Manager and select All Layers > Vias as in figure 21. Drag the mouse to select all the cells under Thru Via To in the DEFAULT row. Type 25 and hit Enter, which copies this value into all cells selected. Close the Constraint Manager and save your board. 4. Run the autorouter from within PCB Editor or export the board to PCB Router as before. This time you should allow routing on both layers, which is the default. You might like to experiment with the directions. Note the routed length and the number of vias; a good design may have none at all, which is a bonus. Remember to gloss or space and mitre the tracks. 5. Import the tracks into PCB Editor if you used PCB Router. Save the routed board under a new name. You must move any vias in inconvenient places, such as that under U3 in figure 20. If you are lucky you may be able to Slide the via but it is often better to rip up the complete track and re-route it by hand. Other tracks must often be moved to create space for the via. • Select the cline or net with the offending via, right-click and choose Delete or Ripup etch from the contextual menu. When you have finished editing your board, add text to both layers of etch to identify them. It would be embarrassing if the top of your board was processed with the bottom of somebody else’s. Finally, plot the finished board in colour.
The board has five free vias, far too many for a board that could be routed successfully with only one layer. The worst via is under U3, which is unacceptable for a home-made via because the wire in the via would obstruct the integrated circuit. (There would be no problem on a commercial board with plated-through holes.) Another via is very close to the trimmer (R8) and it would be difficult to solder this without damaging the trimmer. You would have to solder the via first and keep it neat.
• The pins of the integrated circuits are connected to tracks on both the top and bottom.
This is not a problem if the IC is soldered directly to the board but won’t work if it is in a socket.
• The connectors (J1 and J2) and the trimmer (R8) have tracks only to the bottom of their pins. This is why the via is needed near R8. No tracks run to the top because the symbols for these components have route keepouts on the top, which forbid the router from placing tracks there. The footprints have diagonal shading in PCB Router to show this, visible in figure 16.
2. Remember the Default via padstack when you used the new board wizard? We specified VIA26. Unfortunately this has a bug because another type of via called simply VIA appears in the design and is used wrongly by default. This VIA is much too small so we must get rid of it.
• Select the connect tool and check in the Options control panel that the active and alternate layers are correct.
• Draw out the segments of the track as usual.
• Double-click when you reach the point where a via is needed. A via is inserted and routing switches to the alternate layer.
• Continue routing to complete the track.
I made several changes to the board to get the final version in figure 22.
• The via was moved from under U3 to a clear region of PCB.
• Another via was moved away from R8.
• The via near C1 was eliminated by rerouting the tracks slightly.
• Several tracks were moved from the top to the bottom, which makes the board easier to solder by hand.
• It would have been better to edit the board further so that all tracks leave the ICs on the bottom of the board. This would require extensive rerouting and more vias to be inserted. (Better still, I could have added a route keepout on the top layer of the footprint for the ICs. We have a local library with features such as this to help inexperienced students.) I also prefer to avoid vias in the tracks for power and ground.
