My first manual track routing

MrChips

Joined Oct 2, 2009
30,712
U4 pin-8 CD4017 is GND. Where is the connection?
Are you sure U4 pin-1 is connected correctly?
Where is the GND connection at Power 6-9 volt input?
Did you use schematic capture and rats nest to begin? This would catch routing errors.

Even though a trace meets design rules, I like to give it max clearance on all sides. Where there is space, use it.
Traces should come off pads orthogonally, i.e. straight horizontal or vertical when there are pads on both sides.

Trace at U4-10 to U5-4 is messy and convoluted. Pick the direct route and use vias if you must. Reroute that along with U4-5 to U2-1 and you can probably do it with one cross-over. Keep in mind that one wire jumper is no more difficult to install than one thru-hole resistor.

As a general guideline, I like to keep traces on one side running horizontally and vertically on the other side.
I avoid running traces in between pins if there is an easy route.


20200825 AAC PCB.jpg
 

Thread Starter

christiannielsen

Joined Jun 30, 2019
380
1. U4 pin-8 CD4017 is GND. Where is the connection?
2. Are you sure U4 pin-1 is connected correctly?
3. Where is the GND connection at Power 6-9 volt input?

Even though a trace meets design rules, I like to give it max clearance on all sides. Where there is space, use it.
Traces should come off pads orthogonally, i.e. straight horizontal or vertical.

Trace at U5 pin-7 is messy. Pick the direct route and use vias if you must.
As a general guideline, I like to keep traces on one side running horizontally and vertically on the other side.
I avoid running traces in between pins if there is an easy route.
Thank you very much
1. I was expecting it is connected to a filled pour which is GND. It should do everywhere on the pcb. But maybe I did it wrong?
2. It should be all right. I attach my circuit diagram for you to see.
3. It should be connected to the filled area Pour GND. (admitted. I really havent searched too much about this filled area topic).

Thanks you for your other tips and tricks. Please write again.
 

MrChips

Joined Oct 2, 2009
30,712
A copper pour is done based on the schematic capture. If you don't have that then you will not get the GND pins connected to the ground plane.
 

Thread Starter

christiannielsen

Joined Jun 30, 2019
380
Did you use schematic capture and rats nest to begin? This would catch routing errors.
I am not sure what that means. I think PCBnew (Kicad) shows the air lines (rats nest) by deafault and when I routed tracks the program guided me to the right place/pin. I am not sure what "schematic capture" is.
 

Thread Starter

christiannielsen

Joined Jun 30, 2019
380
Does the decoupling caps work all right when the one pin of the ceramic capacitors are connected to copper pour or should they be deattached the copper pour and routed to the ground pin on the IC's? or is it the same...
 

jpanhalt

Joined Jan 18, 2008
11,087
I would pull this track back a little or reduce the edge clearance for the pour so the ground is contiguous at that point. Same on the other side.

1598385644288.png

That an lead differences in ground potential across short distances.
 

trebla

Joined Jun 29, 2019
542
If you are doing two layer boards i suggest not to draw ground connections for trough hole parts as the ground wires create unnessesary mess for routing process. Instead left ground connections for last stage when you put ground pour on the board. For simpler boards this usually connects all grounds together. If, not then little re-editing is sufficient.

For final inspection use 3D viewer and check overall appearance, are all silksreen items in right place, are components placed reasonably etc.

Some PCB manufactures want you to put text "TOP" in top layer copper and "BOT" on the bottom layer copper, especially chinese one.
 

MrChips

Joined Oct 2, 2009
30,712
Glad to see a much improved layout.

These are my personal preferences:
1) I am not strict about no 90° bends. Use them if it cleans up the layout.
2) I avoid having two traces into one pin (a bused pin). The reason is when trying to a diagnose a problem, sometimes you need to disconnect and/or reroute a signal or power to a pin. It is easier to have to cut one trace to a pin. I would prefer to use T-junctions leading to the pin.

Reroute the power trace at the top of the board so that the traces are below the decoupling capacitors.
(I only highlighted the one trace. Connect them all with a single horizonal trace below the capacitors and use T-branches off the main line.)

The decoupling capacitors centered at the top of the ICs look nice. However, since you are using a ground plane it would be electrically better to offset the capacitor to the right so as to align the capacitor pin with the power pin. The goal is to keep all connections to the decoupling capacitor as short as possible with no bends. I would have chosen to bring the capacitor closer to the IC power pin. If you do this then the power trace has to go above the capacitors.

20200826 AAC PCB.jpg
 

Thread Starter

christiannielsen

Joined Jun 30, 2019
380
Here is my 3rd take on routing tracks.

I have been trying to follow your advice. Im not sure if this try is even better than my last try.

I didn't catch the thing about 90 degrees bends. Were they allowed or were they not?

Screenshot 1: In my last try I connected these tracks shown in the DRC screenshot (GND tracks). But it shouldn't be nessesary right? why arent these three connected to GND Pour? in the 3d viewer they look connected.
1598635875267.png

1598636239933.png
1598636261165.png

Zip-file attached.
 

Attachments

Top