EAGLE question

[bababui]

Hi

I'm making a circuit schematic using EAGLE. There are aproximately 20 points on my board that need to be grounded. Is there a way to have all theese points to be reffered to the common ground point without actually making a separate connection from each point to ground, so that when I create a board file it will automatically make those connections?

thanks

 

[mneary]

Name the signal GND wherever it appears as a net.

Check that this is complete with the command show gnd and confirm that all locations are highlighted.

 

[bababui]

I am still having problems with this.

I connected a GND to Every point on my board that has to be grouded and also to a pin that I want to be designated as the ground pin on my board. Typing in show gnd does highlight all those points, however, when I created the .brd file from my schematic and performed autorouting the ground connections did not show up on the board? What did I do wrong?

I just wanted to let you know that this is my first EAGLE board design and I am learning as I go.

any help is appreciated.

Thanks

 

[justDIY]

use the polygon tool to create (draw) a pour, and then connect the pour to gnd using the name command.

so POLYGON and draw a shape that encompasses the points you want grounded

then NAME 'gnd' and click on one of the polygon borders

now do a RATSNEST to re-render the display and the polygon should fill in everywhere connecting all the gnd pins.

 

[bloody-orc]

show is the eagle files please. then we can get an idea, what you are trying to do.

To connect grounds on schematic you use supply1->GND symbols. They get all connected (reversed T shape). on the board connect all other lines and then make a polygon so that the w hole board is covered with "track" and then rename the polygon also GND. then all GND pins should be connected. Is some remain unconnected, then connect them manually. Also when you are just starting with boarding and EAGLE, then autoroute is something you should avoid. Making them manually will give you99% better results. autoroute is used for either very simple boards or on very big and complex ones.

 

[3v0]

Mneary gave you the right answer.

When you connect two or more points you create a net.

Click on the NAME icon then click on each net you want to be GND and name it GND. They becomes part of the GND net. They will all be connected on the board.

Click on the SHOW icon and click on any net named GND and everything that is connected to it should be highlighted.

Use the INFO icon to find the name of any net.

 

[Ayne]

I have a similar question.

I am using 4511(BCD to 7 Segment) in Eagle Schamatic.. But it has no power supply pins..
How we connect power supply with it??

 

[bloody-orc]

see image above. left column, from botton 4'th. invoke

 

[Ayne]

I am making Main Board in Eagle.
But there is a problem
**broken link removed**
How to connect +5 Volts and ground to IC2(4028) and IC1(4511).

(I will make it's PCB in Eagle)
Thanks

 

[3v0]

Bloody-Orc answered this but let me try again.

On some chps the power and gnd pins are not shown on the symbol used in the schematic. This is because you may want to put them near the power supply section rather then the logic.

Click on INVOKE. It is the icon about the T icon. Then click on IC1 and you will be presented with a menu that lets you select the power and gnd. When you do so you will get pwr and gnd pins for IC1 that you can place anywhere on your schematic.

HTH

 

[Ayne]

Thanks 3V0

Now the problem solved.

 

[justDIY]

if you create a net named Vss (or vdd, vee, vcc, depending), Eagle will automatically connect power / supply pins named the same to that net, so you don't have to expose the additional power pins for the IC (there's a reason they are hidden)

but a lot of times we mix and match chips, some use Vss, some use Gnd. The net ends up getting named one or the other and so eagle won't automagically make that connection.

 

[philba]

but a lot of times we mix and match chips, some use Vss, some use Gnd. The net ends up getting named one or the other and so eagle won't automagically make that connection.

I really wish that eagle would allow synonyms for a net. Thus, for example, you could make Vdd, Vcc and +5V be the same wire. Although that could have problems with mixed voltage systems. Gnd and Vss similarly.

 

[3v0]

I agree.
I want an indicator the shows the number of unrouted traces. Of at least if any exist.

 

[justDIY]

I want an indicator the shows the number of unrouted traces. Of at least if any exist.

Turn off top and bottom layers (1 and 16), leaving pins, pads and unrouted layers turned on. Now you can see any air-wires that were buried under the other more colorful layers.

 

[philba]

The problem with that is that it's really easy to get these tiny little airwires when the pads are off grid. I turn off pads as well.

hit ratsnest - that will tell you how many airwires are left.

 

[3v0]

That is what I do now. Actualy I turn off everything (as doesphilba) but the unrouted layer so I can see the ity bity illegimate ones that hide under the pads.

But I am lazy and would rather have the indicator.

 

[3v0]

hit ratsnest - that will tell you how many airwires are left.

Hey I never noticed that. I got my wish.

 

[bloody-orc]

I just use the track command to see, if it hooks up to any airwires left.... if it does, then I start searching it

But on schematics it is a VERY bad habit to leave Eagle do the Vcc and other power pins connecting... ALWAYS do it yourself to make sure everything is connected and you don't have to start checking the PCB afterwards. it isn't hard to use those supply symbols now is it And it also makes it easier to read the damn schematic afterwards by anyone else, who would like to use it. Also a lot easier to check if it will work. Especially when you post those schematics online (like here to be checked or something).