Two questions; auto router and vias

Am 09.06.2014 18:35, schrieb Olav S. Flaa:

I have two questions:

 

1. Some components like terminal blocks and large electrolyte capacitors

are supposed to be placed directly on the PCB which means that the pins

must be soldered on the bottom layer. When I use the auto router

feature, it makes traces both in the top and the bottom layer. Is there

a way to tell the auto router feature that all connections to specific

components have to be routed in the bottom layer? (What I did as a work

around: Draw a rectangle/circle in the packages top-layer to define the

size of the component, ran the auto router feature and then removed the

temporary rectangles/circles.)

 

2. When I make VIAs on the board, the DRC gives a clearance error

because the top and bottom traces overlap in the VIA-point. This happens

even if the VIA is identical to those made by the auto router feature

(which don't cause clearance error). What am I doing wrong?

 

Thanks for any help!

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/115764

 

1. Autorouter/General-Tab setting N/A into a layer will block the use.

2. Can't say directly but something does not fit the design rules.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Thanks for your reply!

Unfortunately I can't block the top layer, I need to auto route using both the bottom and top layer. But the routing to/from a few specific components has to be on the bottom layer.

1. It would be nice if someone could confirm that this isn't possible if that is the case.

2. This is still a mysterium to me. But I will hopefully figure it out sometime.

Am 14.06.2014 09:57, schrieb Olav S. Flaa:

1. It would be nice if someone could confirm that this isn't possible if

that is the case.

2. This is still a mysterium to me. But I will hopefully figure it out

sometime.

 

 

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/116687

 

Place an area "trestrict" around parts you don't want to connect on top.

Help layer.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

1. Thank you! This is exactly what I needed.

2. I have found what the problem was. I inserted a via and connected one trace from the top layer and another from the bottom layer, both connected to the same net. But the via didn't automatically switch to that net, but was connected to its own separate net. So I had to manually give the vias the same net name as the traces connected to them. I didn't know that a via had its own net. And I don't understand why there was no question similar to when I connect two wires in the schematics view, but I assume there is a reason for it that I'm not capable to understand yet.

On 14/06/14 16:25, Olav S. Flaa wrote:

I didn't know that a via had its own net. And I don't understand

why there was no question similar to when I connect two wires in the

schematics view, but I assume there is a reason for it that I'm not

capable to understand yet.

I suppose I can see how this is confusing, but it does make sense.

First off, understand the purpose of the two editors:

   The schematic editor is used to draw a representation (schematic) of

the function of the circuit. It defines what the circuit is, including

which pins are connected to which others.

   The board editor is used to lay out the physical components and

copper in such a way as to achieve the circuit defined by the schematic.

Now, a consequence of this is that any change to the circuit must be

done on the schematic, not the board. If you connect two nets together

on the schematic, that's considered a change to the circuit and you are

asked how to resolve the change. If you connect two nets together on the

board, that's an error, which will be flagged up by DRC.

So what if you add a via on the board? There could be two reasons - you

might want to run a net through it or you may just be making a hole for

mounting purposes. In both cases there are better ways to do this, but

the important thing is that Eagle doesn't know which you intended.

Either way, the via has a net associated with it as part of its nature,

but the editor doesn't know which net you intended until you rename it.

So it creates it with a newly allocated, unique net all of its own. That

may not even be wrong, in fact.

Hope that helps,

Rob

Thanks for your helpful explaination!

I thought vias were for connecting nets through holes and holes/drills was for making holes for mounting purposes (I read in the help-file that drills are conducting through holes but holes are not). Although I know the purpose of the schematic versus the board and that any changes in the circuits have to be done in the schematic, I didn't realize that this of course has to be the consequence of it:

"If you connect two nets together on the schematic, that's considered a change to the circuit and you are asked how to resolve the change. If you connect two nets together on the board, that's an error, which will be flagged up by DRC."

In addition I didn't know this:

"via has a net associated with it as part of its nature, but the editor doesn't know which net you intended until you rename it. So it creates it with a newly allocated, unique net all of its own."

But now I know :-)

Olav S. Flaa wrote:

I thought vias were for connecting nets through holes and holes/drills

was for making holes for mounting purposes (I read in the help-file that

drills are conducting through holes but holes are not). Although I know

the purpose of the schematic versus the board and that any changes in

the circuits have to be done in the schematic, I didn't realize that

this of course has to be the consequence of it:

"If you connect two nets together on the schematic, that's considered a

change to the circuit and you are asked how to resolve the change. If

you connect two nets together on the board, that's an error, which will

be flagged up by DRC."

In addition I didn't know this:

"via has a net associated with it as part of its nature, but the editor

doesn't know which net you intended until you rename it. So it creates

it with a newly allocated, unique net all of its own."

Placing vias by hand is normally not neccessary.

Vias will be created automatically, in the course of routing an

airwire, whenever you change the layer (middle mouse button or

dropdown layerlist in the tool bar).

Vias will also be generated when you change the layer of a track.

Should it be neccessary to create vias be hand - for instance to tie

GND planes in different layers together, you can use the via command

with the net name as parameter like: "via 'GND".

--

Lorenz

Aha, very useful information, thank's a lot!

It takes A LOT of time to learn complex software like this. Some programs take years to master, I assume Eagle is one of those. Luckily, I only need it for fairly simple audio-circuits.