Placing vias while routing

On 5/5/2010 4:14 PM, Chris wrote:

I am creating my first PCB layout in Eagle and I have placed all of my

parts and created inner power and ground polygon planes and I'm at the

point where I need to start routing.

I am routing power/ground first, and I find that I have to place a via,

rename it to the net name that I need it to be, and then place my traces.

It's a real pain to do, and I'm not looking forward to doing it for my 500+

nets.

Is there a way for me to create a trace and midway through drop a via and

have it automatically have its net name be the same as the trace?

 

 

yes, change layer to the target layer and the via will drop. this can be

done sometimes by clicking the middlemouse button to cycle through the

layers. although i think you may need to click the left mouse before or

after the middleclick to define the point.

On 5/5/2010 4:14 PM, Chris wrote:

I am creating my first PCB layout in Eagle and I have placed all of my

parts and created inner power and ground polygon planes and I'm at the

point where I need to start routing.

I am routing power/ground first, and I find that I have to place a via,

rename it to the net name that I need it to be, and then place my traces.

It's a real pain to do, and I'm not looking forward to doing it for my 500+

nets.

Is there a way for me to create a trace and midway through drop a via and

have it automatically have its net name be the same as the trace?

 

 

ok, left click to locate the via, middleclick to change layer, left

click again to drop via, then escape to stop routing.

"Chris" wrote

I am creating my first PCB layout in Eagle and I have placed all of my

parts and created inner power and ground polygon planes and I'm at the

point where I need to start routing...............

............Is there a way for me to create a trace and midway through

drop a via and

have it automatically have its net name  be the same as the trace?

Route to the point you want your via. and hold the Shift key as you Left

click. This will drop a via with the same name as the signal you are

routing. You then continue routing on the same layer you were on.

If the via/trace is over a polygon with the same name it will connect.

Ratsnest to confirm.

Warren

On Wed, 05 May 2010 16:14:48 -0700, Chris <fongcj.eee@gmail.com>

wrote:

...Is there a way for me to create a trace and midway through drop a via and

have it automatically have its net name  be the same as the trace?

Yes, just start routing, and when you get to where you want to place a

via, while the routing is still active, switch to a different layer

and continue routing.  Eagle will place vias where you changed layers.

You can configure the size and shape of these automatic vias too, or

you can edit them after they are placed.

Robert Scott

Real-Time Specialties

Ypsilanti, Michigan

On 5/5/2010 6:14 PM, Chris wrote:

I am creating my first PCB layout in Eagle and I have placed all of my

parts and created inner power and ground polygon planes and I'm at the

point where I need to start routing.

I am routing power/ground first, and I find that I have to place a via,

rename it to the net name that I need it to be, and then place my traces.

It's a real pain to do, and I'm not looking forward to doing it for my 500+

nets.

Is there a way for me to create a trace and midway through drop a via and

have it automatically have its net name be the same as the trace?

 

 

Hi Chris,

Actually if you are going to route your ground an Vcc signals first

there's actually a very neat trick to have the autorouter do them for you.

For this trick to work, you need to convert your power and ground

polygon planes into supply layers. First Delete the polygon planes next

using the display command select your power and ground layers and make

sure you turn them into supply layers.

Once this is done here's where the cool part begins. In the command line

type

AUTO GND VCC;

This tells the autorouter to only route signals named GND and VCC. Once

the autorouter settings come up, delete all of the optimize runs. Under

the route bus change the maximum number of vias to 9999. These changes

will allow eagle to lay down vias and run all of your ground and vcc

connections straight to your supply layers. You may have to play a

little bit with the cost factors if it doesn't work on the first try.

One note about supply layers is that they are negative layers. If you

draw a trace on a supply layers, the trace is what is going to be etched

away not the surrounding area. It's the opposite of the normal layer

definition.

Hope this helps.

Regards,

Jorge Garcia

cfong wrote on Wed, 05 May 2010 19:14

Is there a way for me to create a trace and midway through drop a via

and have it automatically have its net name  be the same as the trace?

Yes, see HELP ROUTE.

--

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