Doubts about autorouting and polygon filling

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...

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

Don't Be lazy!
Making Boards Is An Art!

Thank you for your reply.

Yes your advice of changing widths also works in some places, but you yourself realised that what I want is to conserve some more space and hence make certain traces occupy some tighter spaces. The thing is, although some power lines should be able to supply upto 1A or something [so I make the traces min 25mils], there are certain connections where just the voltage is required [with very less currents likes 5mA or even lower], as in ICs which just sense the voltage [op-amps]. So I try to make that specific connection a bit thinner and hence occupy tighter spaces and leave me a bit more space for other connecions. It might sound weird.

And yes when it's not possible to autoroute, I do it manually. I'm not completely dependent on it.

And thank you for the advice on changing the width. It works for me when I don't have to physically change the connection mapping.

Thanks.

Thank you for your reply.

I somewhat do it the way you explained. I selectively autoroute my connectoins. But I do the opposite of what you said. I first autoroute the thicker parts and then take care of the thinner parts. If I change the thinner to thicker I might get clearance issues.
Even now I do the autorouting part twice for a connection like I mentioned in my question.

For your reply to my 2nd question, I do the exact same thing - filling the board with GND pour first and then autorouting the remaining first. And then yes I'm too unlucky that I still get unrouted GND connections at some places. But like you said again, I make certain vias and necessary connections again. I was just wondering if there's an easier and "lazier" approach to it.

So in the end, my board becomes a mix of manual and autoroutes. Not a problem though, but just wondered if there's one click setting for my requirement which I might have missed. I'm just a newbie afterall. And lazy.

Thank you.

Ofcourse I whole heartedly agree with you that it is pure art. And I love it.

And I'll take up your advice and try not be lazy in this area.

Thanks..