SparkFun Forums 

Where electronics enthusiasts find answers.

Questions relating to designing PCBs
User avatar
By Chupa
#34873
im trying to design a fairly small board (<2.5in sq) with eagle, not many components(~20), but their most all SMD. When i use the auto router to do the traces i end up with something like 80 vias, which seems like way too much for this small simple board. ive tried optimizing part placement by hand and still seem to end up with a high amount of vias. I think it may be because i messed with the auto router values not knowing what i was doing in there. can anyone recommend some values i should be using in there (route and optimize tabs and what not). im using the batch PCB service so im on a 8mil grid.
User avatar
By leon_heller
#34878
I wouldn't bother with the Eagle autorouter, it has a very poor reputation. The one supplied with the Pulsonix PCB software that I use is excellent, but is a fairly expensive option.

Leon
By rpcelectronics
#34883
Are you limited to having all parts on the same side of the board? If not, consider placing any non crucial, low profile parts on the opposite side. This would be mostly resistors and caps. This can sometime reduce your number of vias. I'm not suprised by the numbers though. I have had larger board with that many parts with a high number of vias. I use Eagle as well and personally, I like the autorouter. Some people think its a real pig, but it really does a decent job for me.
User avatar
By Chupa
#34884
rpcelectronics wrote:Are you limited to having all parts on the same side of the board? If not, consider placing any non crucial, low profile parts on the opposite side. This would be mostly resistors and caps. This can sometime reduce your number of vias. I'm not suprised by the numbers though. I have had larger board with that many parts with a high number of vias. I use Eagle as well and personally, I like the autorouter. Some people think its a real pig, but it really does a decent job for me.
I was just supprized that one of the traces changed board sides 4 times before reaching the destination on the same side! I have is set up as if i were doing a mostly through hole board, Horizontal runs on one side, Vertical on the other. maybe i should try again with that off and just let it do its own thing.

I have access to Utiboard but i have never really used it much because sparkfun recommends and has tuts for eagle, and batchpcb seems to prefeer that as well. maybe ill try that
By Andrew02E
#34905
I have yet to see the Eagle autorouter produce something worthwhile. I used it once on a board with a billion nets, give or take a few. Even then, I spent a whole day cleaning it up.
If the autorouter is switching layers multiple times on one trace, try bumping the cost of vias way up (ie. to 99) or even limiting the maximum number of vias. That might help, or it might not. Like I said, routing boards by hand in Eagle seems to be much quicker and cleaner.
By Philba
#34934
when I first started using eagle, I really wanted the autorouter to work for me. I finally gave it up and started manually routing. It's really not that hard and you will get a significantly better board for the effort.

2.5 sqin and 20 components isn't that hard. Make a copy of your project and give it a shot. Use a ground polygon on both the top and bottom. Then start routing. I think you'll find it not that bad.
By winston
#34965
I don't use Eagle, but I agree on autorouting - it's overrated. I manually route all my boards. You're more likely to think of the consequences of how traces are routed that way, too. I recently read an article by a professional who also suggested that autorouters should be used very sparingly.
User avatar
By leon_heller
#34971
It depends on the autorouter, some do a very good job. I just tried the Pulsonix router on a board I had previously routed manually (no vias), and it completed 100%, using the default settings, without any vias! I don't think that anyone could identify the autorouted one.

With some designs manual routing just isn't viable because of their complexity.

Leon
User avatar
By bigglez
#35069
Chupa wrote:im trying to design a fairly small board (<2.5in sq) with eagle, not many components(~20), but their most all SMD. When i use the auto router to do the traces i end up with something like 80 vias, which seems like way too much for this small simple board.
Greetings chupa,

A lot depends upon the pad count of the parts in your design. Are there 20 passives with two pads each or twenty SOICs with dozens of pads?

Care to post your EAGLE sch file (after running ERC) so we can see what you're attempting to do?

Comments Welcome!
By rr_pilot
#35143
The eagle autorouter really isn't all that bad, you just need to know how to use it. First thing I do is start by giving the router as many choices as possible.

1) Change the routing direction to '*'
2) Change the routing grid to something appropriete, I have found after many trial and error a routing grid of 0.1 mm with traces from 8mil - 12mil.

For some reason eagles router seems to be alot slower then other routers i've used but with 0.1 mm grid then its not to big of a deal anyways.

I've played around alot with changing the settings in the optimization passes with little change in the overall result. The most effective way of reducing vias in eagle is selecting a appropriete routing grid and the placement of your parts.

my 2 cents...
By rpcelectronics
#35240
rr_pilot wrote:The eagle autorouter really isn't all that bad, you just need to know how to use it. First thing I do is start by giving the router as many choices as possible.

1) Change the routing direction to '*'
2) Change the routing grid to something appropriete, I have found after many trial and error a routing grid of 0.1 mm with traces from 8mil - 12mil.

For some reason eagles router seems to be alot slower then other routers i've used but with 0.1 mm grid then its not to big of a deal anyways.

I've played around alot with changing the settings in the optimization passes with little change in the overall result. The most effective way of reducing vias in eagle is selecting a appropriete routing grid and the placement of your parts.
Yeah, I really agree with just about everything you said. The autorouter has a lot to think about as it lays traces, rips them up and looks for a better route (although some don't belive that it does this :D)

I noticed the really slow routing on a 0.1mm grid and I do agree that grid has a LOT to do with the effitiancy of the autorouter. I typically route on a 10 mil grid for most projects. Funny thing is, I do all of my measuring and placing in mm, but I always switch over to mils and set the grid to 10. This seems to help.

As for placement of components, you hit the nail on the head. Paying attention to where you place a resistor that is tied to an IC or whatever makes all of the difference in the world. If a cap is tied to two legs of an ST202 and I place them each at opposite ends of the board, you can bet your *** you'll end up with a bunch of vias when the autorouter tries to get from point A to point B. Strategic placing will reduce this sort of thing immensely. I have seen cases where someone had a project with 20 or so caps and resistors and they wanted the board to look nice, so they just lined them all up and pretty. Sure, that looks nice, but now the traces to get from these to all points of the board is now bloated out of whack and you end up with tons of vias, a crowded mess of traces and more than likely noise or other issues introduced into the design.

Play with the autorouter and you'll find you can do many things to make it work better for you.
long long title how many chars? lets see 123 ok more? yes 60

We have created lots of YouTube videos just so you can achieve [...]

Another post test yes yes yes or no, maybe ni? :-/

The best flat phpBB theme around. Period. Fine craftmanship and [...]

Do you need a super MOD? Well here it is. chew on this

All you need is right here. Content tag, SEO, listing, Pizza and spaghetti [...]

Lasagna on me this time ok? I got plenty of cash

this should be fantastic. but what about links,images, bbcodes etc etc? [...]