Unrouted connections

Hi

It sounds like your PCB is not fully routed so the report you see is to be expected. You can generate gerber files anytime regardless if the pcb is fully routed or not.

When your PCB is complete re-run the status. If you see "Unrouted Connections" this means you have nets not connected. Proceeding to create a finished pcb will mean your board will come back with floating pins !

Not good. "Don't ignore any warnings" Check a few times before going to fab. Also run a check on the gerber files ! 

All the best

Paul.

Actually, the design and routing is completed. What remains is the use of  fanout  for all my unconnected nets and connections-all of those remaining must connect to the ground plane (top layer) as the one that follows:

To my understanding from all I have read in the  Allegro® User Guide: Routing the Design  (c:/Cadence/SPB/doc/algroroute/chap2.html#1035250) - Ch.2-Component Fanout,

So the question is: is creating FANOUT for all thes component pins actually required for the proper finalizing of the design? Should I perform any other step?

Thanks again!

Regards,

Andreas

Andreas,

Fanout is typically used to fanout multi pin BGA components so as to aid in routing. Fanout is not required in any design, you don't have to use it. The only requirement of a design is if a net exists then that net is connected.

Since you have a ground plane on the top layer you can either re-pour the ground plane again and it should automatically connect to your components ground nets, assuming you gave the ground plane a net of ground.

The other option is to manually route each ground connection from a component pin to the ground plane. "Run DRC Checks" when your board is complete !

Best regards

Paul 

Hi Paul,

Thanks for answering again, it is clear now - it is obvious that I do not need the fanout.

I used Shape Add-> [Etch=Top, Type=Dynamic copper, Assign net name=0] and the output is as follows:

It seems that as expected all 0V (GND) Pin of all Symbols are actually connected automatically to the Ground Plane. Only DRC remains.

Seems to be close to finishing!

Regards,

Andreas

Hi Andreas

Well very good it appears you are getting the hang of things. Don't forget to provide enough clearance between your shape and your clines (traces) & component pins. You can also do things like add voids to shapes to make things a bit neater and provide more clearance.

Here is an example of a shape ( gnd ) with voids added. The component pins are connected manually because it was neater than doing a system wide dynamic tie in.

You can see the components R1, C1, R3 connected into ground. In the area around these components there is a shape void. Look at the menu item "Shape > Manual void cavity"
to do something like you see in the picture if that is what you are after. Notice around J3 the pink line. That is the outline of the void which is carving up the plane. 

Also as I mentioned above you want to have enough clearance between your shapes - Traces - Pins so that the dynamic shape does not flood to close, 25 mil or more clearance is a good starting value. On the bottom of my board there is also another ground plane. The vias next to the components tie both planes together.

The shape editor in allegro is very very good, lots of possibilities exist. You can even do logos !

hope this info helps you out.

All the best

Paul