Two questions; auto router and vias

Question

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!

autodeskguest · Accepted Answer

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

autodeskguest · Answer

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

autodeskguest · Answer

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