EAGLE Central Forums
Where the EAGLE community meets. Sponsored by Stratford Digital.

Home » CadSoft Support Forums » eagle.support.eng » track width change
track width change [message #170350] Tue, 02 May 2017 03:24 Go to next message
Messages: 20
Registered: August 2016
Junior Member
Eagle (7.7.0) had me in a corner yesterday, couldn't work out why the auto router wouldn't connect power and ground to a TQFP package, it showed air wires for the omitted connections.

After some playing with the device, gnd@1, gnd@2, append, any/all etc. it dawned on me that if air wires were being drawn, the device and schematic must be OK, it has be something board related causing the problem

It was, 20mil default track width good, 40mil power tracks bad, too wide for TQFP pins.

My solution, auto route with 40mil power, then change to 20mil power and run the auto router again, works a treat, if not very elegant.

My question, is there a correct/better way to change a track's net class to achieve this?

Re: track width change [message #170351 is a reply to message #170350] Tue, 02 May 2017 04:06 Go to previous messageGo to next message
Douglas Wong
Messages: 59
Registered: October 2013
I suppose you could create a separate net for thin power and connect the 2 power nets with a zero ohm jumper. Instead of a physical jumper maybe you can create a part with 2 SMT pads - a big one and a small one, but they are overlapping at one end, creating a short.

To view any images and attachments in this post, visit:
Re: track width change [message #170352 is a reply to message #170350] Tue, 02 May 2017 10:32 Go to previous messageGo to next message
Messages: 239
Registered: February 2014
Senior Member

Well, you have, I would say at least two points to see:
1. Recommendations for circuit board layouts by the component manufacturer
2. PCB rules from the circuit board manufacturer what they need for their machines.
These parameters must be used to configure your network classes.

The values "20mil",,,"40mil" are fictions, ideas, "but not real", ...not for TQFPs.
You can route with 20 or 40 mils, but I suggest make the pwr as a pwr-plane - most important -> the GND as GND-plane.
The signal wire you can route with 20mil, but what ist needing by current thru the wire or can you route between the pins?
That are some questions to have clearing up before routing the board.
A signal wire normally does not need 20mil because it just sends very low current signals, but you need to see high frequency rules.
// routing grid, placing grid, footprint of the devices, dimensions, distances, (mounting) holes, temperature, high- or low frequency, bouncing?, ringing?, noise?, and more ....

Then, if you have your design rules then you can it register in the Eagle in the design rules and net classes.
net class 0 can have e.g. 1mil (default 0 mil)- but, can the PCB manufacturer handle this small wire?

Best Regards,

To view any images and attachments in this post, visit:
Re: track width change [message #170353 is a reply to message #170350] Tue, 02 May 2017 11:08 Go to previous messageGo to next message
Messages: 604
Registered: March 2015
Location: UK
Senior Member
Hi Ken,

Changing your net class rules so you can finish the routing isn't really the right way to do it in my opinion. Imagine, you come to make another change some weeks/months/years from now and you forget your changed the net class rule for the power. You press go on the auto router and it routes in a power trace much narrower than intended which for whatever reason goes unnoticed. You could end up with a problem on your board. Now, this may not be an issue for this situation because we have no knowledge of your circuit or requirements, but in general I would avoid doing things that could lead to errors at some point in the future.

Now, what Gerald says above, using power/ground planes is good advice, but sometimes this isn't practical, especially if you are trying to use 1 or 2 layer boards, but it's worth noting, but this could also be an issue with other high current nets other that just power/ground.

What I would say is that you maybe should reset your expectations for what the autorouter should be used for in reality. It is very rare that the auto router should be used for completely routing a board with no manual intervention, EAGLE's autorouter, as with pretty much every other vendors equivalent just aren't good enough to be able to do a complete board and have the finished result that would be 100% satisfactory, unless the board is really very simple e.g. a backplane with pretty much straight 1-to-1 routing.

I think of the auto router more of a routing assistant, so you use it to quickly put in sets of nets which are easy and obvious to route and would otherwise just be a long winded click fest to do manually. It's actually rare that I would do this as I pretty much route everything manually, but on occasion I do if it's obvious that the router will do a good job and it'll save significant time.

So back to your issue, I would sort out the breakout of the IC's manually first to get the traces out, decoupling caps connected up correctly with short traces etc and then try the auto router for the power/ground, then any other important signals and then finally the remainder of the board. I'd then go tidy up anything that was obviously messy from the autorouter and manually finish off anything it was unable to achieve.

Best Regards,


To view any images and attachments in this post, visit:
Re: track width change [message #170370 is a reply to message #170350] Wed, 03 May 2017 13:17 Go to previous message
Messages: 20
Registered: August 2016
Junior Member
Hi all and thanks for the replies.

I know of the 0 Ohm R trick to isolate nets but never thought of refining it to a pair of small, shorted pads. It does result in physical separation where the net size change happens, which is something I try to avoid with bypasses on supply lines.

My 20 and 40mil track width are a hangover from days of DIY board making. I do a quite a bit of soldering and desoldering on professionally made prototypes and 5mil tracks and minimal pad sizes don't stand up too well, also a 40 mil track will cope with the occasional accidental over current far better than 5mil. I consider the PCB fabricator's design rules a minimum.

Rachael, "Changing your net class rules so you can finish the routing isn't really the right way to do it", couldn't agree more, that's why I said it wasn't very elegant and asked for the correct way.

Maybe I should explain my situation, I'm not a professional, I've made the occasional board now then over the last forty or so years. Back in the day it was sticky pads and black tape in assorted widths (what was it called?) , much easier now with a bit of computing power and Eagle.

I appreciate what you say about the auto router not being perfect but for what I do it does a far better job than I can. My last board was a dozen 74 type packages in a random logic design along with a few opto isolators and about 60 pins of connectors. Now, just the number of possible combinations of package positions and track routing is far more that I can cope with. My approach is to roughly group components together, run some power and ground and the let the auto router have ago, followed by some close inspection and assessment, and if I don't like the result I start adjusting.

I don't have to meet exacting standards, no GHz RF running around or sub nano second propagation delays to worry about, it's not "mission critical" but that doesn't mean I'll be happy with a rubbish job.

I understand there is art in a good layout as there is in any engineering endeavour and please, please don't interpret my comments as in any way trying to denigrate the professionals who prefer to route manually, it's just that it's a skill I don't have. If I was to do ten hours a day for ten years I might start to get somewhere but as I've probably done less than 200 hours in five years I'm not going to get there.

I'll take the advice offered in your last paragraph, I see it as basically an incremental approach, let the auto router do a bit, fix/tidy up by hand, repeat until done, as opposed to put the go button and hope it finishes. Fortunately I recently discovered the power of Eagle's command line input as opposed to WIMP input.

Previous Topic: Library for JST PH connectors
Next Topic: DXF to Eagle Conversion
Goto Forum:

Current Time: Mon Sep 25 13:23:48 GMT 2017