Eagle NC Via

Community PCB Design
1

Hi,

I have a 2 layer board I am working on, it is my first PCB and am having some problems with Eagle.

The problem I am having at the moment is that some of the vias have an X over them, and some dont. I assume the X to indicate a no-connect, but am not really sure. What does it mean? Also, how do I get rid of them, or convert the others to have them? I can provide a screenshot if required.

Another problem, not major, but anoying enough to make me think I am doing something wrong; if I select the ‘route’ tool, then set it to layer 16, then click on a via and try to route, it changes back to layer 1/top. To lay track on the bottom layer, I need to start to lay track on the top, then change the dropdown to bottom. It doesn’t do this all of the time though. Is this normal or am I missing something?

Is there a way to move component labels around?? I can only seem to move the name of a single resistor, trying with any of the other labels selects the nearest track.

Thank you for any help, I am having great fun laying out the board.

Bee

2

Barney:
The problem I am having at the moment is that some of the vias have an X over them, and some dont. I assume the X to indicate a no-connect, but am not really sure. What does it mean? Also, how do I get rid of them, or convert the others to have them? I can provide a screenshot if required.

Sorry, can’t help with this one. I’ve often wondered about that myself.

Barney:
Another problem, not major, but anoying enough to make me think I am doing something wrong; if I select the ‘route’ tool, then set it to layer 16, then click on a via and try to route, it changes back to layer 1/top. To lay track on the bottom layer, I need to start to lay track on the top, then change the dropdown to bottom. It doesn’t do this all of the time though. Is this normal or am I missing something?

This is a peculiarity with Eagle. What I do is start the trace and move the mouse to the drop down menu to change the layer (yes, the trace will follow the mouse off screen). Don’t know why this happens, but it’s something you’ll have to accept.

Barney:
Is there a way to move component labels around?? I can only seem to move the name of a single resistor, trying with any of the other labels selects the nearest track.

I’m assuming you’re using the “Smash” tool first? If so, left click close to the label you want to move. If the wrong item is selected, right click until the label is selected and then left click again and move.

3

To get rid of the X things, try hitting the ‘Ratsnest’ button (or Tools->Ratsnest). That’s the first suggestion that comes to my mind. Let me know if that doesn’t get rid of them. If not, my guess is that Eagles displays them because a trace/via is close enough to look connected (and would probably be connected after fabrication), but they’re not on the same coordinate.

Also, just so you don’t get surprised, ratsnest will shorten your ‘unrouted’ lines (airwires?) to the closest possible connection and will fill any planes you have drawn.

4

what does DRC tell you?

5

Philba:
what does DRC tell you?

Philba,

The DRC tell you if the board design meets the set rules on the design rules. Thinks like clearance, size ,etc.

James L

6

Barney:
The problem I am having at the moment is that some of the vias have an X over them, and some dont. I assume the X to indicate a no-connect, but am not really sure. What does it mean? Also, how do I get rid of them, or convert the others to have them? I can provide a screenshot if required.

Greetings Barney,

The ‘X’ in a board layout indicates a zero length airwire.

This can happen for a variety of reasons, and although

the board might be manufactured correctly the design

data base is in error (and won’t pass DRC).

Quoting from the EAGLE on line help:

Zero length airwires
If two or more wires of the same signal on different routing layers end at the same point without being connected through a pad or a via, a zero length airwire is generated, which will be displayed as an X-shaped cross in the Unrouted layer. The same applies to smds that belong to the same signal and are placed on opposite sides of the board.
Such zero length airwires can be picked up with the ROUTE command just like ordinary airwires. They may also be handled by placing a VIA at that point.

For best design (and your peace of mind) you should

correct every zero length airwire before running the

CAM job (to create Gerbers).

Over time you will learn how to prevent these, or at

least how to kill them. It helps to temporarily nudge

the offending via a bit and then I turn off all layers

and turn on layer 19 (Unrouted) to inspect for zero

length airwires. Many times these can be removed by

grouping the entire board and using the Delete command.

EAGLE complains (as this operation can’t be

back-annotated) but when you redraw the screen the

X should be gone and a new airwire indicates the

offset via that can be moved back to the desired

position.

EAGLE is very literal, but it is better to have false

positives than release a design with errors.

Comments Welcome!

7

Barney:
Another problem, not major, but anoying enough to make me think I am doing something wrong; if I select the ‘route’ tool, then set it to layer 16, then click on a via and try to route, it changes back to layer 1/top. To lay track on the bottom layer, I need to start to lay track on the top, then change the dropdown to bottom. It doesn’t do this all of the time though. Is this normal or am I missing something?

Greetings barney,

You’re not missing anything, EAGLE has a rule about

which layer to route when an airwire is selected.

Quoting from the on-line help:

Selecting the routing layer
When you select an airwire, the initial layer in which to route is determined by considering the objects at the starting point as follows:
·if there is an object in the current layer, the current layer is kept
·else one of the layers of the objects at that point will be taken

So a lot depends on where you pick up the airwire

when you start a manual route.

If you start a manual route and the outline is the

wrong colour (layer) you can quickly select the

desired layer with the mouse centre button (if

available) or dragging the routed trace off the

board to the drop-down layer menu.

Comments Welcome!

8

Barney:
Is there a way to move component labels around?? I can only seem to move the name of a single resistor, trying with any of the other labels selects the nearest track.

Greetings Barney,

Attributes of Objects (components) such as the text

are grouped in EAGLE until the SMASH command

separates the various elements.

Once SMASHed the text, reference and any other

text can be relocated, changed, or modified.

Quoting from the EAGLE on-line help:

The SMASH command is used with elements in order to separate the text parameters indicating name and value from the element. The text may then be placed in a new and more convenient location with the MOVE command.
Use of the SMASH command allows the text to be treated like any other text, e.g. CHANGE SIZE, ROTATE, etc., but the actual text may not be changed.
A “smashed” element can be made “unsmashed” by clicking on it with the Shift key pressed (and of course the SMASH command activated).

Typically I Smash and remove the component values

(part numbers), leaving only the name (designator).

EAGLE uses “>Name” and “>Value” properties for each element.

Examples:

Name C1, IC2, R1, etc.

Value 100n 25V, ATmega8, 1K0 1% (Respectively).

I change the text size and font and reposition the

designator to suit the board design (not all library parts

are built with the same text attributes). I use the SFE

“silk-gen.ulp” to process all the text once the board

is finished and passes DRC.

Comments Welcome!

9

Hello,

Thank you very much!

I was smashing the components, but I didn’t know about the right-click to change to the next one.

I have just finished my first PCB design :smiley: It is completely crammed onto the board, the next step for me will be to place components on the bottom layer as well as the top :shock:

A couple of final questions though; the DRC check shows 7 errors, all ‘restrict’ where I am running track from the circuit to 7 different pads (for external connections). If anyone knows if this is what should happen please let me know.

Finally - I have seen schematics made in eagle that have a fancy boarder around them, allowing things such as title,date, author etc to be added. Does anyone know of any user scripts to do this?

Once again, thank you very much for your help!

Barney.

10

Barney:
Finally - I have seen schematics made in eagle that have a fancy boarder around them, allowing things such as title,date, author etc to be added. Does anyone know of any user scripts to do this?

It’s a library element called “frame”. Look in frames.lbr.

11

Barney:
the DRC check shows 7 errors, all ‘restrict’ where I am running track from the circuit to 7 different pads (for external connections).

Greetings Barney,

Can you post the EAGLE *.sch and *.brd with this error?

(Or PM me).

It is possible that your pad symbol has a keepout or

other restriction that trips the DRC error.

Comments Welcome!

12

If you turn on your restrict and keepout layers, it’ll display the restrict/keepout areas. A lot of parts have restrict/keepout areas included (SMD resistors and capacitors, crystals, etc.), so if you didn’t have those layers turned on when you were routing your PCB, you may have accidentally crossed one of these areas.

13

Hi,

Thank for the info about frames - I wasnt expecting it to be a component!

With regards to the errors, there is a ‘keepout’ region. I had another look through the libraries to see if I could find a replacement and found another one that works. Before I was using a ‘pad’ from holes.lbr called MOUNT-PAD-SQUARE-3,2. Changing this to a ‘WIREPAD’ component works like a charm!

Thanks for the help everyone!!

Barney.