Connecting two separate nets to one junction.

Cant you create a net with different size traces?

On 01/07/14 17:02, Brian Wilkins wrote:

I'm trying to connect two different nets to one junction.  Each nets

carries separate trace sizing due to amp draws from components.  How can

I connect the two nets to one junction with out combining the nets? I

would like to keep the nets separate to minimize trace size on the final

pcb.

This is a VFAQ! (Is there an FAQ page for this newsgroup anywhere?)

Basically, if two nets are connected then they're the same net. To keep

them separate you need to connect them only through a component. But

since Eagle knows nothing about what components actually do, it's quite

happy to accept a device which just wires things together. The normal

trick is to create a device whose symbol is two pins connected together

and whose package is two (SMD) pads coincident. This will create DRC

errors but you can accept them and they go away.

Brian Wilkins wrote on Tue, 01 July 2014 12:02

I'm trying to connect two different nets to one junction.  Each nets

carries separate trace sizing due to amp draws from components.  How

can

I connect the two nets to one junction with out combining the nets?

You can't.  Everything in a net is connected, which is not connected to any

other net.  Remember that what order a line on a schematic connects to

different pins has nothing to do with what order the trace on the PCB will

eventually connect the same pins.

As Rob has already said, you create separate nets for the traces you want

different classes for, then connect them with a component that is just

copper on the PCB.  This is exactly what my "shorts" library is for.  It is

included in my Eagle Tools release at

http://www.embedinc.com/pic/dload.htm.  They look like slightly thickened

short lines on the schematic.

The downside of this method is that you'll get lots of annoying DRC errors

due to the overlaps between the pads in the short packages.  Maybe some day

Eagle will finally have the ability to be told to ignore DRC error wholly

within specific packages pre-approved for that purpose.  For now you'll

have to approve all the errors.  If you move one of these short packages

around on the PCB, then you'll have to approve them all over again.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Actually, the link above is http://www.embedinc.com/pic/dload.htm  As

shown, it includes the "." as part of the link which breaks it ... ain't

technology wonderful??

mikey

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Thank you for the help.  I was able to use a generic component between the net connections.