High Current Traces

On 6/9/2012 2:59 PM, Dave Wills wrote:

Hi,

 

I'm a new Eagle user, but I suspect this is actually a more complicated question.

 

I have traces that will carry up to 2 amps.  Those traces also control various FETs and other signals.  If I set that net node to the trace width for the high current, all of the net gets set to that width and I don't have room to route my board.  I've already re-arranged all my components so that the wide traces are short and the pins near each other.  I've even gone from 4 layers to 6 layers.  (The board routes just fine with 4 layers by 7 mil traces.)

 

I don't see a way to set the width of signals before routing, and after routing is too late.  One idea is to isolate the low current part of the net from the high current with a 0 ohm resistor, then after routing fill in will a trace.  But even that seems a little clumsy.

 

I'm considering going to thicker copper layers so that I can reduce the trace width, but I haven't tried that yet.

 

Does anyone have any ideas on how I might solve this problem?

 

Thanks,

 

Dave

 

Help -> Net Class

You can create net classes with all the traces in the same class having

various common properties including width and clearance from other

conductive elements.    Good for high(er) current and also high voltage.

Jim

Hi Jim,

I've done that.  I have a separate net class for the high current traces.  The problem is one net goes to a few high current nodes (output of high current supply, connector, resistor, FET) but it also goes to a bunch of places that are not high current (but still the same node).  So the high current pins on the node need to be connected with wide traces, but the signal level pins do not.  If I allow all of the pins to be high current traces, I can't get it to route.

That's why I said I could split the high current and signal level pins on the net with a 0 ohm resistor.  Then Eagle wouldn't automatically make all the traces high current traces.  But that sounds like a clumsy solution.  Seems better to make the copper thicker then make all the traces less wide.

Thanks for the suggestion.

Dave

On 6/9/2012 4:37 PM, Dave Wills wrote:

Hi Jim,

 

I've done that.  I have a separate net class for the high current traces.  The problem is one net goes to a few high current nodes (output of high current supply, connector, resistor, FET) but it also goes to a bunch of places that are not high current (but still the same node).  So the high current pins on the node need to be connected with wide traces, but the signal level pins do not.  If I allow all of the pins to be high current traces, I can't get it to route.

 

That's why I said I could split the high current and signal level pins on the net with a 0 ohm resistor.  Then Eagle wouldn't automatically make all the traces high current traces.  But that sounds like a clumsy solution.  Seems better to make the copper thicker then make all the traces less wide.

 

Thanks for the suggestion.

 

Dave

 

You can override the default trace width using the Change -> Width tool.

    This will allow you to manually specify segment by segment the width

of a trace.

Jim

Dave Wills wrote:

Hi Jim,

 

I've done that. I have a separate net class for the high current

traces. The problem is one net goes to a few high current nodes

(output of high current supply, connector, resistor, FET) but it also

goes to a bunch of places that are not high current (but still the

same node). So the high current pins on the node need to be connected

with wide traces, but the signal level pins do not. If I allow all of

the pins to be high current traces, I can't get it to route.

 

That's why I said I could split the high current and signal level

pins on the net with a 0 ohm resistor. Then Eagle wouldn't

automatically make all the traces high current traces. But that

sounds like a clumsy solution. Seems better to make the copper

thicker then make all the traces less wide.

 

Thanks for the suggestion.

 

Dave

If you have organised the positions of the high current points then you

should manually route them with the desired width and then let the auto

router do the remaining unrouted nets narrower.

Using the autorouter entirely, you could route with the setting you mention.

At this point all you wide traces are complete. Then ripup every thing

except the wide net name. Then ripup any remaining wide traces that should

be narrow. Next change the class width to narrow and run the autorouter

again

HTH

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

My apologies if I'm being dense.

I don't appear to be able to change the width on any unrouted traces.  Am I missing something?

Manually routing some nodes doesn't seem like a good option.  If I tweak anything and need to start over, it takes a lot of time.

I could route the wide traces first, but I can't rip some of the traces on a node and leave others alone, then auto routed the ripped wide traces with a smaller width.  At least, not without a lot of manual work.  Seems I'd need to route wide traces, rip the ones that don't need to be wide, then change the width of the signals on that net, and finally continue routing with the new widths.  Again, this is a lot of manual work.

To give an idea, here are my high current nodes:

N$61  C21      1        P$1        3 *** up to 1 amp
         C22      1        P$1        3 *** up to 1 amp
         L3        2        2          3 *** up to 2 amps
         R24      1        P$1        3 signal level
         R25      2        P$2        3 signal level
         R26      C        P$2        3 *** up to 2 amps
         R27      2        P$2        3 signal level
         U4       9        VON        3 signal level

N$60   C19      2        P$2        3 signal level
         L3        1        1            3 *** up to 2 amps
         U4       11       SW         3 *** up to 1 amp
         U4       12       SW         3 *** up to 1 amp
         U4       13       SW         3 *** up to 1 amp
         U4       14       SW         3 *** up to 1 amp
         U4       15       SW         3 *** up to 1 amp
         U4       16       SW         3 *** up to 1 amp

N$62   Q8       4        S          3 *** up to 2 amps
         R26      A        P$1        3 *** up to 2 amps
         U5       6        -IN        3 signal level
         U7       6        -IN        3 signal level

N$63   Q10      4        S          3 *** up to 2 amps
         Q11      4        S          3 *** up to 2 amps
         Q8       1        D          3 *** up to 2 amps
         Q8       2        D          3 *** up to 2 amps
         Q8       5        D          3 *** up to 2 amps
         Q8       6        D          3 *** up to 2 amps

You can see that there are low current (skinny traces) mixed in with high current (wide) traces.  Even though the traces that need to be wide are near each other, the signal level traces get routed as wide traces.  When these need to go through vias and inner layers, it doesn't leave enough room for the rest of the signal level traces.  (Note that I have created some polygons around some of the signals, for example U4 11 - 16.  That does help routing somewhat.)

And then, consider the same problem when you look at GND.  I have a similar number of high current traces.  Though I have a ground plane, I need to specify some vias as larger than others into the ground plane in order to carry the current.

I'm starting to think that maybe Eagle isn't useful for boards with mixed trace widths and high density.  I might be better off having a professional layout firm do the last step.

Thanks for reading.

Dave

On 10/06/2012 09:10, Dave Wills wrote:

My apologies if I'm being dense.

 

I don't appear to be able to change the width on any unrouted traces.  Am I missing something?

 

Manually routing some nodes doesn't seem like a good option.  If I tweak anything and need to start over, it takes a lot of time.

 

I could route the wide traces first, but I can't rip some of the traces on a node and leave others alone, then auto routed the ripped wide traces with a smaller width.  At least, not without a lot of manual work.  Seems I'd need to route wide traces, rip the ones that don't need to be wide, then change the width of the signals on that net, and finally continue routing with the new widths.  Again, this is a lot of manual work.

 

To give an idea, here are my high current nodes:

 

N$61  C21      1        P$1        3 *** up to 1 amp

          C22      1        P$1        3 *** up to 1 amp

          L3        2        2          3 *** up to 2 amps

          R24      1        P$1        3 signal level

          R25      2        P$2        3 signal level

          R26      C        P$2        3 *** up to 2 amps

          R27      2        P$2        3 signal level

          U4       9        VON        3 signal level

 

N$60   C19      2        P$2        3 signal level

          L3        1        1            3 *** up to 2 amps

          U4       11       SW         3 *** up to 1 amp

          U4       12       SW         3 *** up to 1 amp

          U4       13       SW         3 *** up to 1 amp

          U4       14       SW         3 *** up to 1 amp

          U4       15       SW         3 *** up to 1 amp

          U4       16       SW         3 *** up to 1 amp

 

N$62   Q8       4        S          3 *** up to 2 amps

          R26      A        P$1        3 *** up to 2 amps

          U5       6        -IN        3 signal level

          U7       6        -IN        3 signal level

 

N$63   Q10      4        S          3 *** up to 2 amps

          Q11      4        S          3 *** up to 2 amps

          Q8       1        D          3 *** up to 2 amps

          Q8       2        D          3 *** up to 2 amps

          Q8       5        D          3 *** up to 2 amps

          Q8       6        D          3 *** up to 2 amps

 

You can see that there are low current (skinny traces) mixed in with high current (wide) traces.  Even though the traces that need to be wide are near each other, the signal level traces get routed as wide traces.  When these need to go through vias and inner layers, it doesn't leave enough room for the rest of the signal level traces.  (Note that I have created some polygons around some of the signals, for example U4 11 - 16.  That does help routing somewhat.)

 

And then, consider the same problem when you look at GND.  I have a similar number of high current traces.  Though I have a ground plane, I need to specify some vias as larger than others into the ground plane in order to carry the current.

 

I'm starting to think that maybe Eagle isn't useful for boards with mixed trace widths and high density.  I might be better off having a professional layout firm do the last step.

 

Thanks for reading.

 

Dave

 

In your schematic, connect the non_high current nets to the high current

nets with a 0 ohm resistor, they'll have a different name.

Specify the adequate width to the high-current nets using class, route

as usual, then remove the resistor and connect directly.

there is some work in the schematic.

HTH

Hi Morosh,

Yes, that is where I started in my original post.  I tried doing it and it got complicated.  Maybe I'll try again.

Thanks,

Dave

Hi Dave,

If you insist in 0-ohm "bridges", you might (most likely, according to your description how this is becoming complicated) want to add more than one split-resistor per net.

To get a good estimation about number of 0-ohm resistors needed, perform the following steps: (1) run autorouter, (2) highlight trace of interest, (3) count number of trace branches mixing high and low current flows. These joints are initial candidates for your 0-ohm resistors location.

BTW: I prefer (at least) partial manual routing.

Best wishes,  Ivan.

Hi Ivan,

Thanks for the suggestions.  Yes, that's pretty much what I thought

needed to be done.  But as my initial report said, I'm a new user so

I'm still learning a lot.  One thing that stops me from manually

routing is I ran into a roadblock adding vias.  I couldn't figure out

how to make the corresponding hole in the ground plane to run the via through.

In the meantime, I figure I can go to 2 oz copper and thinner

traces.  I'm pretty close in routing everything (3 wires out of 350),

so figure I can get there with some care.

Not sure about some manual routing.  I don't know enough about Eagle yet.

Thanks again!!!

Dave

OK, final post on this.  After a bunch of tweaks, I've gotten everything to route with this last problem.

I have a QFN24 package that has 6 output pins which together provide up to 5 amps.  Each pin has a width of 0.25 mm.  The 6 pins are overlaid with a polygon which is connected to one of my high current traces.  My high current trace is 0.5 mm.  The router creates traces which are the width of the wide netclass trace, 0.5 mm, and even though there is a polygon connecting the pins, the router runs traces between all the pins.

Here's the problem.  At the end points of the polygon connecting the 6 pins, the 0.5 mm traces extend past the 0.25 mm pads, violating the spacing to the next pins.  I can't change the width of the pins or the width of the traces.  Do I rip just those traces then route manually?

Thanks,

Dave