6
\$\begingroup\$

I am just about done with a layout. But Eagle says I have 23 air wires left. It turns out they are little tiny ones, e.g. where traces overlap, like this one:

enter image description here

There is a tiny yellow dot where the two traces overlap pointed to by the arrow. Is there a way to join these traces together to eliminate this? Or do I have to delete one trace, and extend the other one? I also have this happen where a trace is connected to a pin -- I will get a little air wire and can't seem to get rid of it.

If I verify that all my remaining air wires are of this type, can I just send the board out to fab as is, since all of the traces seem to overlap?

\$\endgroup\$
  • 1
    \$\begingroup\$ 'eephphphph' <- sound of sucking air through teeth. At best, the fab is going to run the DRC, so any warnings left over are just going to cause the board to bounce and cause you grief. At worst, I've had some verrrrry strange behaviour where something that 'should' have been OK came back with missing copper due to an incompatibility with the way two different products handled an edge case. It's a wonder these tools work at all, don't provoke problems by sending out something that is complaining for a reason you don't fully understand. \$\endgroup\$ – Neil_UK Dec 10 '16 at 7:00
  • \$\begingroup\$ 'can't seem to get rid of'. Have you imported a component with an imperial grid, and you're gridding to metric, or vice versa. That's caused me all sorts of untidiness in the past. \$\endgroup\$ – Neil_UK Dec 10 '16 at 7:04
  • \$\begingroup\$ What happens if you run the auto router? - just a guess to get rid of this. \$\endgroup\$ – sweber Dec 10 '16 at 7:32
  • \$\begingroup\$ Name that small segment of net with the via to match the net you are trying to connect. I presume you added the via using the via tool, in which case it is assigned to some random new net like N$10. \$\endgroup\$ – Tom Carpenter Dec 10 '16 at 10:11
  • \$\begingroup\$ @TomCarpenter I checked using right-click Properties, and both the via and the small segment of the net have the same name as the large segment, JTAG_RST_B. \$\endgroup\$ – tcrosley Dec 10 '16 at 13:15
8
\$\begingroup\$

This typically happens when the system of units of the grid is changed between metric and imperial during routing. Even with very fine sub-divisions, it is quite impossible to align the endpoints of two tracks drawn in different units exactly.

One behavior of EAGLE is that when you start a new track, the start-point snaps to the next position of an air wire (you need to hold SHIFT to let a track start just under your mouse pointer), but the end point will never snap to anything than the grid.
There's just one hint that you indeed hit the correct position: There's no new line segment sticking to your mouse pointer.

Due to this, I'd recommend to stick with one unit for the grid, changing not more than the number of sub-divisions.

If a part does not fit onto the grid, don't route tracks into the pads of this part, as they will not snap to the precise positions of the pads. Instead, route tracks out of the pads, since then they will snap to the correct position, and after the next kink, the track is on-grid again.

Since you are convinced the board is OK, you could just send the board into production, but this could lead to queries and delays. And as said in the comments, you could get unexpected results if for example the line ending type changes somewhere during the conversion from EAGLE format to whatever the manufacturer uses.

So, it's better to get rid of the airwires, and I'd suggest to let the auto-router do the job.
Be a little careful, the auto-router will not change its track with to match the width of the existing stubs. If it uses a too large width, you get knobs in your tracks, which can lead to clearance errors. On the other side, if the stubs don't overlap, you can get too thin track segments.

|improve this answer|||||
\$\endgroup\$
  • 1
    \$\begingroup\$ It may happen even if you stay with the same unit of the routing grid. If you use parts with a pin pitch of 2.54 mm and 1 mm in the same design you have to switch between routing grids of 0.635 mm and 0.25 mm for instance. To route the tracks out of the 2.54 mm pitch part, you use the 0.635 grid and for the 1 mm pitch part the 0.25 mm grid. But even in this case it is possible route all tracks without angle errors, isolation gap errors and tiny air wires. I have done such a design with eagle some years ago. But I needed a transition area for the change from one grid to the other. \$\endgroup\$ – Uwe Dec 12 '16 at 16:53
1
\$\begingroup\$

If you carefully use the ripup tool you can back the trace up one segment at a time. If the ripup tools makes the whole route an airwire, you need to use the backspace to go back one click. Then try to land to the center of the pad.

|improve this answer|||||
\$\endgroup\$
0
\$\begingroup\$

I found several little air wires on my layout and worked out that they were actually representing connections between layers. I put in a via and hey presto!

|improve this answer|||||
\$\endgroup\$
  • \$\begingroup\$ Welcome to stackexchange. How does your situation become an answer to this question? \$\endgroup\$ – StainlessSteelRat Apr 13 '18 at 19:31
  • \$\begingroup\$ The question was about little air wires and how to remove them. Grid inconsistency is one but air wires also appear if you are need a connection between layers, say a ground plane. At least that is something I have experienced. \$\endgroup\$ – andrew buckley Apr 14 '18 at 21:30
-3
\$\begingroup\$

Likely this (your PIX) is a nothing.

I always Print my PCBs because what appears to be connected on paper, will be connected on the PCB.

Attach a COMMENT SHEET to your PCB work order, so the operator can understand your intent.

I find Eagle to be like an obstinate pig, there are more friendly packages out there. SPRINT LAYOUT software has some neat features, such as allowing a .BMP or .JPG drawing to be the background of your layout page.

And use software appropriate to the task. There are five PCB packages on my companies network but I wouldn't use Cadence except for more sophisticated jobs.

1:1 printouts of your handiwork allow you to physically look at the final product before you commit to production. Insert the physical component's wires through the paper so you have a realistic reproduction.

Autorouters are often a joke, they come up with the most inappropriate 'solutions'! I usually don't even link the schematic to the layout screen, but that is after years of experience. My first piece of software was from Racal-Redac, which dates me, and I have laid many kilometres of black tape on mylar sheets!

|improve this answer|||||
\$\endgroup\$
  • 1
    \$\begingroup\$ This doesn't in any way answer the question. \$\endgroup\$ – Tom Carpenter Dec 22 '16 at 16:21

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.