Board Size Marker

Type "display all;" and hit the enter key to see if the outline shows up.  If it does, the layer was turned off.  If it doesn't show up, you've probably deleted it.

To hide or show layers, click on the layer settings icon just below the information icon, or you can enter "layer" on the command line...

BTW, to go back to your previous layer settings you can type "display last" after you use the "display all" command.  (You probably don't want all of the layers displayed at the same time...)

Thanks. I tried this but nothing changed, the board boundary is still gone so I guess I deleted it. Is there any way to resurrect it?

Depending upon your settings, there should be several backup files in your project directory.  Open the EAGLE control panel and go to the Options menu, then to Directories... and look at the bottom entry to find where your projects are stored.  Navigate to that directory, and you should see some files with the endings .b## and .s## (they will be numbered in order, they won't have the standard .brd and .sch endings); those are backup files.  The first thing I would do would be to create a new directory and copy all of the backup files into that directory.  Then you can rename the board files one at a time so that they end in .brd, and open each one in EAGLE until you find the one with the board outline.  Then you can either look at the properties and recreate the outline in the newest file, or you can open the newest file and then copy and paste...

Good luck!

This sounds like it will be at the very least time consuming and at worst very risky to my current project.

Is it possible to

"Group All"

"Copy"

"Delete Board"

"Create New Board"

"Paste All"

Will that work?

I THINK I fixed it. I created a new project, checked the "Properties" of the board outline ("wire", "width = 0, "continuous", "Layer 20") and reproduced them on my board. I now have a board outline starting at the origin point. I hope this does it.

Thanks

As I said I've "fixed" the board outline and hopefully its correct. I've finished cleaning up the board and I'm now outputting the Gerber files. I keep getting warnings about the top and bottom Ground polygons and the GBT file is 7.8MB. The project is very simple consisting of an Arduino ProMini, a wireless module, some screw terminal blocks, a few discrete components. The board is about 3in x 1.9in, 2 layer with top/bottom ground planes.

Does this file size seem reasonable?

On 6/25/2014 12:53 PM, John Steele wrote:

As I said I've "fixed" the board outline and hopefully its correct. I've

finished cleaning up the board and I'm now outputting the Gerber files.

I keep getting warnings about the top and bottom Ground polygons and the

GBT file is 7.8MB. The project is very simple consisting of an Arduino

ProMini, a wireless module, some screw terminal blocks, a few discrete

components. The board is about 3in x 1.9in, 2 layer with top/bottom

ground planes.

 

Does this file size seem reasonable?

That's way too big. The warnings your getting refer to the width of the

polygons. Basically you want to make sure that your polygons have a

non-zero width.

The reason is that polygons are made by laying wires of the given width

right next to each other, if you have zero width wires then you have an

infinite number of wires in the polygon. NOT GOOD.

In reality there's no such a thing as a zero width wire, in EAGLE zero

width means the smallest width EAGLE can represent (0.003um if I recall

correctly). Such a thin wire will generate huge amounts of data and

that's why your GBT file is 7.8MB.

Check your polygons and make sure they have a non-zero width and then

try running the CAM processor again.

hth,

Jorge Garcia

I fixed the "wire" size and re-exported ... made an enormous difference my export file size is 46k now

Thanks