PCB with Eagle Cadsoft!! Help!!

[geppou]

Can anyone tell me how I can connect with autorouter all vias on Eagle using double layer PCB but  the connection to the pins of components are only on the bottom side?(because i can't solder all type of component on the top but on the top can running vias)
Sorry for posting here this question but i can't find answer on web..help me please

[CrossRoads]

Post your files, lets see what the problem is.
The autorouter usually creates the vias needed to connect top & bottom traces.

[geppou]

The problem is that I want al vias(and others) indicate with arrows on the bottom and not on the top because with a circuit like this I can't solder on Top of PCB

[DeepZ]

From the question i assume you are going to make the boards yourself, otherwise the holes would be through plated and you would only have to solder on the bottom.

You could place a restrict rectangle or polygon on the top of the board where you do not want any tracks. So this would be on top of the pins of the connector. This way the autorouter knows it cannot put a trace there on the top and is forced to use the bottom only.

See this picture, where i placed a top-restict (layer 41) rectangle on the top connector, which forces the auto-router to only place vias where i can reach them.

Hope this helps,
Guido

[CrossRoads]

All those green mounting holes will be plated on both sides of the board.
I'll try to remember to take a picture of a similar board at home and post so you can see that.
If you use Edit:View Layers and turn off all but top layer & pads & vias, then do the same for bottom layer & pads & vias, you can see where copper will be left.
You could also use File:CAM processor and create gerber files and review the top & bottom layers to confrm.
If you click Download here
http://imall.iteadstudio.com/open-pcb/pcb-prototyping/im120418001.html
and download the DRC and CAM files, you can run the Design Rule Check to make sure your traces are all manufacturable, and then use the CAM file for gerber creation to see just what will be made. I use the free viewer from www.viewplot.com to look over the gerber files.

[geppou]

Hope this helps,
Guido

Yes this is the perfect answer to my question.Thank you very much!

All those green mounting holes will be plated on both sides of the board.
I'll try to remember to take a picture of a similar board at home and post so you can see that.
If you use Edit:View Layers and turn off all but top layer & pads & vias, then do the same for bottom layer & pads & vias, you can see where copper will be left.

Yes I use this function and with it you can made a PCB with Vias and Pad on Bottom and on Top but the problem is that they aren't connect in an Home made PCB and for example if I want to put a 28 pin socket for the ATmega I can solder only the pad on bottom and if a connection start from the top of the  pin of the ATmega this connection isn't connect with the pin of the ATmega and that is wrong

Can you answer me for another question please?
I want to cover all PCB bottom and Top with GND and to do this I cover the area with a polygon and rename it with GND name..but a warning occur and advise me that " Signal name 'GND' already exist! use the NAME command to combine signals" and then the PCB's area is cover but NOt connected to GND...How can I solve this?

[CrossRoads]

Odd about the Gnd planes - I do that on every board and do not have that problem.
You will not have much bottom Gnd plane if All your traces have to end up there.
Post your actual eagle files, I can try it when I get home.

Your board seems pretty wide open - why can't you solder those pins on both sides before putting other components around them?
Unless you are using sockets, I could see access being difficult then.

[geppou]

thank you for your Help and for your site to make PCB (please could you link me other sites you know for compare?).
I attach the schematic that it is complete and the board that it isn't complete if you want to take a look...thanks!

[DeepZ]

Can you answer me for another question please?
I want to cover all PCB bottom and Top with GND and to do this I cover the area with a polygon and rename it with GND name..but a warning occur and advise me that " Signal name 'GND' already exist! use the NAME command to combine signals" and then the PCB's area is cover but NOt connected to GND...How can I solve this?

I think you are changing the name of the polygon using the info (i symbol in the toolbar) tool? That indeed will generate this error.
To change the name of the polygon use the name (r2 over resistor symbol in the toolbar) tool , click on the polygon and change the name to GND. It may ask if you want to merge the net with the GND net, which we indeed want.

That you can use the ratsnets tool to show the ground-plane.

Hope this helps,
Thanks,
Guido

[CrossRoads]

I right-click to bring up the list of commands and select Name from there.
Don't think I ever click i button except by accident.

[geppou]

Yes..the error was that I modified the name from the properties of the polygon and not from the option name that it was also simply...stupid XD...thank you very much to all

[CrossRoads]

Okay, tweaking your design some (12 mil traces vs 25), and assuming a double sided board still, adding a couple of ground vias, I get a design like this.

[geppou]

Thanks for your time but with a home made pcb I think that is difficult to sold on top some components like for example the crystal...I used 25 mil for via because i'm afraid to lost vias during the process to do the physical sircuit board but I can try with this configuration....different is if I use site like that  you link to me but I learn to create the file to send they....Do you know a guide to learn this?

[geppou]

Another question sorry
How can I do the operation you can see on the photos? I try to delete the GND for connect a blu wire but I don't know how I can do....can anyone help me another time please?

[CrossRoads]

I think this might do it for you.
Need a few jumpers to complete all the signal paths, shown here as the red wires.
All the components are soldered from the bottom.
I'll leave it to you to make any traces wider if you want them to be.
I made the vias for the jumpers the same diameter holes.