How do you choose a routing grid value?

Questions relating to designing PCBs

Moderator: phalanx

How do you choose a routing grid value?

Postby snarflemike » Sat Jun 20, 2009 1:29 pm

I'm using Eagle right now, but I'm sure my question is not Eagle-specific. When using an autorouter, what are the guidelines/tradeoffs in selecting a value for the routing grid?

Mike
snarflemike
 
Posts: 15
Joined: Thu Jun 11, 2009 11:06 am
Location: Florida

Postby leon_heller » Sat Jun 20, 2009 1:32 pm

When using autorouters the grid should be set quite small. I use 5 mil for the Pulsonix autorouter, as a rule, and it does a very good job. The Eagle autorouter is rubbish, BTW.

Leon
Leon Heller
G1HSM
User avatar
leon_heller
Support Volunteer
 
Posts: 5734
Joined: Sun May 01, 2005 11:20 am
Location: St. Leonards-on-Sea, E. Sussex, UK.

Re: How do you choose a routing grid value?

Postby davep238 » Sat Jun 20, 2009 6:19 pm

snarflemike wrote:I'm using Eagle right now, but I'm sure my question is not Eagle-specific. When using an autorouter, what are the guidelines/tradeoffs in selecting a value for the routing grid?

Mike

If you have a low density board (mainly DIPs), then a 25-mil grid may work. Otherwise, I'd go for a 10-mil grid, or possibly a 5-mil grid. Basically, try different grid and see what works best for your board. I've noticed that EAGLE's auto-router (AR) leaves a bunch of wiggly lines when the grid is too small. It looks like it "changes its mind" quite a bit with small grid settings. I've gotten tired of cleaning up after EAGLE's AR, so I rarely use it anymore. If nothing else, running EAGLE's AR will give you some ideas of how to manually run traces.

I think that most people "know" that EAGLE's AR is lousy. There is an on-line AR that works with EAGLE and is much better, but I can't remember the URL (sorry). I've played with a demo of Pulsonix and was really impressed, especially with its AR. I don't have the money for Pulsonix ($3K - $5K) or enough freelance work to justify buying it, so I'm sticking with EAGLE for now.
-Dave Pollum
programmer / digital designer
PCBs designed for low cost
davep238
 
Posts: 157
Joined: Thu Dec 13, 2007 8:51 am
Location: Burke, VA, USA

Postby leon_heller » Sun Jun 21, 2009 1:41 am

Pulsonix actually uses the Electra autorouter:

http://www.connecteda.com/

It is available for Eagle. It might look expensive, but it's much cheaper than other autorouters.

Leon
Leon Heller
G1HSM
User avatar
leon_heller
Support Volunteer
 
Posts: 5734
Joined: Sun May 01, 2005 11:20 am
Location: St. Leonards-on-Sea, E. Sussex, UK.

Postby gussy » Sun Jun 21, 2009 3:22 am

Try routing with a 5mil grid. I also find that increasing the "cost" of vias makes for a much better auto-route. That being said, I never auto route. Period.

Try the autorouter, then rip it up and try yourself. Practice and you will get better ;)
gussy
 
Posts: 460
Joined: Fri Jul 28, 2006 5:25 am

Postby rpcelectronics » Thu Jul 02, 2009 9:59 am

A 5mil grid is ok, but just make sure the board house you are working with accepts that.

Gold Phoenix is a min 7 mil grid, unless you want to pay more. So, by default, I route everything at a 7 mil grid to make sure I meet that requirement.
Jason Rausch - Amateur Radio Callsign: KE4NYV
RPC Electronics, LLC
www.rpc-electronics.com
rpcelectronics
 
Posts: 184
Joined: Thu Oct 05, 2006 3:17 pm
Location: Greenbackville, Va.

Postby leon_heller » Thu Jul 02, 2009 10:09 am

I don't understand how the routing grid is relevant to the board supplier.

Leon
Leon Heller
G1HSM
User avatar
leon_heller
Support Volunteer
 
Posts: 5734
Joined: Sun May 01, 2005 11:20 am
Location: St. Leonards-on-Sea, E. Sussex, UK.

Postby rpcelectronics » Thu Jul 02, 2009 10:42 am

leon_heller wrote:I don't understand how the routing grid is relevant to the board supplier.


By setting the routing grid less than the min spacing allowed by the PCB manu, there is the chance for two traces to either be spaced below this min clearance or the clearance with another part/pad could be less. Thus causing it to fail the min requirement. Such as GP's 7 mil min.

Its just a fail-safe thing I do to prevent it.
Jason Rausch - Amateur Radio Callsign: KE4NYV
RPC Electronics, LLC
www.rpc-electronics.com
rpcelectronics
 
Posts: 184
Joined: Thu Oct 05, 2006 3:17 pm
Location: Greenbackville, Va.

Postby leon_heller » Thu Jul 02, 2009 11:20 am

The software I use won't let me make errors like that.

Leon
Leon Heller
G1HSM
User avatar
leon_heller
Support Volunteer
 
Posts: 5734
Joined: Sun May 01, 2005 11:20 am
Location: St. Leonards-on-Sea, E. Sussex, UK.

Postby gussy » Thu Jul 02, 2009 4:25 pm

leon_heller wrote:I don't understand how the routing grid is relevant to the board supplier.

Leon

leon_heller wrote:The software I use won't let me make errors like that.

Leon

I am pretty sure your right there. I have used a 5mil grid in the past many times on boards with 7 or 8 mil clearance. EAGLE is smart enough to not violate the DRC when autorouting.
gussy
 
Posts: 460
Joined: Fri Jul 28, 2006 5:25 am

Postby TheDirty » Thu Jul 02, 2009 4:50 pm

Wouldn't a 7mil grid violate a 7mil space requirement if it didn't know what it's doing? 7mil grid would mean that the traces were spaced centre to centre 7mils apart, making the space between smaller.
Mark Higgins
TheDirty
Support Volunteer
 
Posts: 657
Joined: Sun Jan 04, 2009 8:06 am
Location: Toronto, ON, Canada

Postby leon_heller » Thu Jul 02, 2009 10:37 pm

Even a 1 mil routing grid won't violate the 7 mil track spacing requirement. The track spacing will always override it.

Leon
Leon Heller
G1HSM
User avatar
leon_heller
Support Volunteer
 
Posts: 5734
Joined: Sun May 01, 2005 11:20 am
Location: St. Leonards-on-Sea, E. Sussex, UK.

Postby signal7 » Sat Jul 04, 2009 5:41 am

If you load the .dru file before you run the autorouter (or specify the requirements in the design rule check before you run the auto router), Eagle won't violate those requirements. You could autoroute with a 1 mil grid and the results should still pass the design rule check when you're done.
signal7
 
Posts: 177
Joined: Fri Nov 07, 2008 7:52 am


Return to PCB Design Questions

Who is online

Users browsing this forum: No registered users and 1 guest