1. Is there a route to the ground plane? In general you must add vias from you component layer grounds with a short track - then the plane layer can connect to the ground net.
2. It sounds like you have been routing with a different set of rules to those set by the DRC. I suggest you edit the DRC rules to suit your PCB manufacturer.
3. I don't use the autorouter so cannot help there.
If you are still stuck the PCB files would be useful.
Keith
I cannot see a brd file - just a screenshot. I cannot see any unconnected nets on there but it is difficult to view. Also, you haven't flooded the ground planes anyway. Maybe if you post the brd file it will be easier to see what is happening.
Keith
You seem to have a short circuit from your GND pins on two connectors on the right hand side. A 0.1mm track runs right through several pins on the top layer.
You grid is set to 0.001" which seems rather small.
All your tracks are ridiculously small - 0.1mm. Apart from being an unsuitable width for a lot of functions (too small) you will have to pay a premium to get someone to make it.
There are no unconnected grounds after doing a ratsnest. Have you turned on "Ratsnest processes polygons" in the "Set|misc" menu?
Your board edges are not at right angles - probably as a result of using a 0.001" grid for drawing.
For making a break off portion of the board you should use routing (the milling layer on Eagle). Your PCB manufacturer will not make a board with drills like that - the drill will break.
Your DRC errors are probably mostly due to the tracks which are too narrow. Other errors are:
short circuits (overlap)
drill size
- drill distance - the break off section mentioned above
- dimension - items too close to the board edge
- clearance - tracks too close to other tracks/pads
I would suggest you rip up all the tracks, re-draw the outline with a sensible grid (e.g.1mm), don't use the autorouter, remove the break off holes and then run a DRC. Get a clean DRC before you start. Then set some sensible wire and grid and start manual routing. Run the DRC very regularly to start with and fix errors as you go. That way you will learn and be able to do the DRC less often.
Keith.
Well, there are definitely no unrouted nets when I ratsnest. When I load the board initially there are two unrouted traces but they are spurious - they do not end on a component or trace. So, they disappear when I ratsnest. They are probably there because you have deleted some spurious tracking.
By the way, you should also use a sensible grid when placing components - it makes it a lot easier to route.
It should easily route on 4 layers. Even 2 layers is possible but as you should probably have a decent ground plane I would use 4 layers.
One other point on the schematic - you have used a "bus" a few times but as you haven't drawn it going anywhere it doesn't really do anything. Normally buses are used to show a block of connections from one place to another without needing to show the individual nets, which gets messy. You have relied on the net labels for the connections so the bus doesn't show anything. If you want to use a bus then your would run the bus from the radio module to the GPIO connector to show where the connections are going.
You could probably have fitted all the circuit on the first sheet.
Keith.
I will look later, but one quick check with a footprint is to print it out 1:1 on paper and put the component on it.
Keith.
Now its a rectangle. Actually it is a separation of an extension part from main board. I would like to manufacture it in such a way that I can break that part from the main board later on if I want to. I'm not sure if it is a rectangle, how I can break it from the main design?You have put holes on the milling (route) layer 46 - it should be a rectangle.
If I increase my grid to 0.05" then it wouldn't allow me smooth movement of components and track. Anyways how does grid selection gonna make any difference to design and manufacturing? Isn't grid is only for our convenience?Your grid is still tiny - 0.005". I wouldn't normally tun with a primary grid less than around 0.05" on a board like that. The secondary grid can be smaller for tricky routing.
Now default track width is 0.01" and I used 0.015" for power tracks and 0.005" for critical routing.Your defualt track width is 0.016". If you used something like 0.01" then you could pack more tracks in. You would normally use wider ones for power.
How can I add these crossing pads in schematic? I dint find any option to add it in schematic.overlap errors - you have tracks crossing pads which have been added to the PCB but not to the schematic so there is no corresponding connection (e.g. across the PCB break-off). Normally you would make sure everything on the PCB is on the schematic.
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?