Doubts about autorouting and polygon filling

Question

Hello.

Thank you for listening to my doubts.

I've two questions mainly related to routing in the board designs.

1. I usually design boards which have a lot of connections. Being a lazy person, and with the awesome autorouting capabilities of EAGLE, I prefer to autoroute everything. Now I've many connections which should have different widths, like the power lines should be thicker [20 to 25mils] while normal I/O wires can go down to 16 or even 12mils. What I do in that case is create different netclasses for different types of connections [set different widths, via diameters, and clearance values], and then autoroute it. It works absolutely perfectly.

Now in my current board design, I've a situation where I want the very same connection [net] to be 20mils at certain places and 12 mils at certain places. Using netclasses I can either set it to 20 or 12mils at a given time, not both. So I can only autoroute that connection at 20mils first, then remove [ripup] the part that should be 12mils and autoroute the same connection again [with 12mils netclass] to get the autoroute to route at 12mils.

So is there any other way I can solve this situation by routing the very same connection [net] at two or more different widths at different physical points on the board at the same time? That way I'll only have to autoroute the whole board just once. Any help will be appreciated. By the way, the autorouting capabilities of EAGLE are simply amazing. Thank you EAGLE team for that functionality.

2. Thank you again for taking the time to read my doubts. My second doubt regarding board designs is about the polygon filling [copper pouring] part. I usually design double-sided boards with both sides polygon fillings of Ground planes, and occasionally 5V or 3.3V fillings.It might be a stupid question but should I fill the layer before starting my routing, or do it after I've routed the board 100%?

Having already mentioned above that I usually use the autoroute capabilities of EAGLE, if I autoroute my boards after polygon filling, I get a message that "polygons may have fallen apart".

When I fill the board before routing, I need to make proper vias at different points so that both layer fillings are shorted at all points. And it also makes the routing part tougher for me or the autorouter [maybe I'm wrong].

On the other hand, the opposite is much easier, i.e. routing the board first and then doing the pouring.

I personally feel that the copper pouring should be done before the routing, because doing it after everything has been routed doesn't improve the connections according to me. Again, any advices on this topic will be greatly appreciated.

Thanks a lot for even taking the time to go over my doubts.

Any inputs will be greatly appreciated.

And thank you team EAGLE for this lovely piece of software. Without you all I would have given up PCB designing. You all make it easy.

Rahul Sharma.

autodeskguest · Answer

On 1/03/2014 7:51 a.m., Rahul Sharma wrote: Hello. Thank you for listening to my doubts. I've two questions mainly related to routing in the board designs. 1. I usually design boards which have a lot of connections. Being a lazy person, and with the awesome autorouting capabilities of EAGLE, I prefer to autoroute everything. Now I've many connections which should have different widths, like the power lines should be thicker while normal I/O wires can go down to 16 or even 12mils. What I do in that case is create different netclasses for different types of connections , and then autoroute it. It works absolutely perfectly. Now in my current board design, I've a situation where I want the very same connection to be 20mils at certain places and 12 mils at certain places. Using netclasses I can either set it to 20 or 12mils at a given time, not both. So I can only autoroute that connection at 20mils first, then remove the part that should be 12mils and autoroute the same connection again to get the autoroute to route at 12mils. So is there any other way I can solve this situation by routing the very same connection at two or more different widths at different physical points on the board at the same time? That way I'll only have to autoroute the whole board just once. Any help will be appreciated. By the way, the autorouting capabilities of EAGLE are simply amazing. Thank you EAGLE team for that functionality. First, ensure you have read Chapter7 of the manual and chapter 15 of the tutorial. "Autorouter: A Brief Example". Both in the Docs folder of your installation. You probably have. To answer your question #1. No. Eagle cannot read your mind. You would have to give it some clues about which area needs what and there is no way to do that for a one pass solution. Your design will dictate the approach to take. The first is to Autoroute (AR) at the smallest width and then selectively widen the traces that you want wider. click click click. Just as Doug said. What you can do is to run the Autorouter (AR) twice. Place restrict rectangle/polygons on the tRestrict and bRestrict to keep it from routing in those areas. Perform one pass at the desired width for the signal then remove the restrict areas and run the AR again, with the settings for the other width . It will complete the routing using this new value. There is a disadvantage here that the portion that is routed actually becomes satisfied without considering the portion that is not so in some cases routing the remaining portion may be less efficient. So the method you spoke of will be better. It all depends on your design and the space available for the traces. 2. Thank you again for taking the time to read my doubts. My second doubt regarding board designs is about the polygon filling [copper pouring] part. I usually design double-sided boards with both sides polygon fillings of Ground planes, and occasionally 5V or 3.3V fillings.It might be a stupid question but should I fill the layer before starting my routing, or do it after I've routed the board 100%? Having already mentioned above that I usually use the autoroute capabilities of EAGLE, if I autoroute my boards after polygon filling, I get a message that "polygons may have fallen apart". When I fill the board before routing, I need to make proper vias at different points so that both layer fillings are shorted at all points. And it also makes the routing part tougher for me or the autorouter . On the other hand, the opposite is much easier, i.e. routing the board first and then doing the pouring. I personally feel that the copper pouring should be done before the routing, because doing it after everything has been routed doesn't improve the connections according to me. Again, any advices on this topic will be greatly appreciated. Thanks a lot for even taking the time to go over my doubts. Any inputs will be greatly appreciated. Read AUTO in the HELP There it explains you can exclude a signal from the AR. So try this: Exclude the signals that can get a connection/interconnect via the polygon copper pour. AR the remainder and then do the ratsnest for the excluded signals (Likely ground, GND). If you are in luck all GND pads/SMD will be connected (non isolated). Check for remaining airwires. This is only good when you dont need to consider the ground loops in the copper pour as in mixed signal designs. You may have to preempt the result and drop a via in strategic places. From the above and what you read elsewhere, you will see why designers will manually route and if they use the AR it is used selectively. HTH Warren

AnalogNotes · Answer

I don't use the autorouter, but why not just use the "change width" command and just click on the parts you want to be the different width? Or do you want the autorouter to take a different path with the thinner traces? (I'm not sure I understand why you change trace widths though...) I'll have to let someone else help you with #2. I route things by hand, using various combinations of "ratsnest;", "rip @;", and "drc;" myself with the occasional "display none 19;" to show airwires and "display last;" to go back...