finishing touches in routing

Any tips during the finishing touches in routing?

If you have thin tracks (<25 thou) then it’s nice to add a “chamfer” to any “T” junctions, thus eliminating any 90 degree angles. This makes the track more physically robust, and prevents any potential manufacturing etching problems. But most importantly, it looks nice.

Check that you have any required mounting holes on the board. Keep mounting holes well clear of any components or tracks. Allow room for any washers and screws.

Minimise the number of hole sizes. Extra hole sizes cost you money, as the manufacturer will charge you based on not only the number of holes in your boards, but the number of different hole sizes you have. It takes time for the very high speed drill to spin down, change drill bits, and then spin up again. Check with your manufacturer for these costs, but you can’t go wrong by minimising the number of hole sizes.

Double check for correct hole sizes on all your components. Nothing is more annoying than getting your perfectly laid out board back from the manufacturer, only to find that a component won’t fit in the holes! This is a very common problem, don’t get caught out.

Ensure that all your vias are identical, with the same pad and hole sizes. Remember your pad to hole ratio. Errors here can cause “breakouts” in your via pad, where the hole, if shifted slightly can be outside of your pad. With plated through holes this is not always fatal, but without a complete annular ring around your hole, your via will be mechanically unreliable.

Check that there is adequate physical distance between all your components. Watch out for components with exposed metal that can make electrical contact with other components, or exposed tracks and pads.

Change your display to “draft” mode, which will display all your tracks and pads as outlines. This will allow you to see your board “warts and all”, and will show up any tracks that are tacked on or not ending on pad centers.

If you wish, add “teardrops” to all your pads and vias. A teardrop is a nice “smoothing out” of the junction between the track and the pad, not surprisingly, shaped like a teardrop. This gives a more robust and reliable track to pad interface, better than the almost right angle between a standard track and pad. Don’t add teardrops manually though, it’s a waste of time. But if your program supports automatic teardrop placement, feel free to use it.

Hope this helps!

To add to above points, ensure that the PCB is USER FRIENDLY. Main issue we face while prototype testing is the access to test points. Add legends for Test points wherever possible. And in cases where a test point cannot be added, add a legend to one of the vias on that signal. and make sure all legends for test points are on TOP side of the PCB.

Make sure to check via tenting (that is: via covering by soldermask). You don't want to scrape soldermask off from some via to test voltage because you forgot to remove tenting. On the other hand there are some metal parts (like various connectors) which may cause a short circuit if vias underneath are not tented.

Add somewhere to clip your oscilloscope ground for testing and remember to add some sort of PCB reference to identify it.

Keith

It is nice to design a board in such way, that potential transporting system on assembly line will not touch solder pads. Otherwise it may contaminate solder pads or damage components on board. That is why you should implement a component free zone of about quarter of an inch at board sides.

You can omit that if your board is assembled as a panel. In such case panel boundaries (or frame, or whatever it is called) serve as holding area.

If your board is small then only reasonable way is to design it as a panel, because handling very small pcb's in many cases costs extra (simplest reason being that assembly line operator has to operate more boards which translates to more time needed for whole process and as a result - higher cost)