I am trying to prepare a circuit for printing at a manufacturer; ShenZhen2U, for the first time. But, a stray island is appearing on the bottom layer of the board.
Here has been the procedure:
I downloaded and installed theShenZhen2U EAGLE Design Rules.
I loaded them into the DRC.
Before I run the DRC, the stray island does not show up.
After I run the DRC, the stray island appears.
The following functions do not remove the island:
Trash Can
Rip-Up
Redraw
Ratsnest
Orphans = Off
I have done my “homework” and have not come across the answer. So, I would appreciate your help with removing the stray island. I would also like to know if I may ignore the stop mask errors. Any other general suggestions would also be welcomed.
Well, you know it’s on the bottom layer, you can turn off all other layers and see if you can get to it. The DRC should not have put anything into the board. If all else fails, go into your Eagle documents folder and rename a board and sch file with the right extensions. Find the files that have an earlier time before the DRC check.
I realized what you suggest and started working on that idea… I believe the item is stuck in the isolation that is on the PIC chip pads… I just haven’t dug deep enough to get to it… You have made me realize that I need to turn off the pads… Maybe that will give me access… If you zoom in, you will see that the orphan is in wire form…
Okay, I completely removed everything that was on the schematic and, then, I updated the ratsnest on the board. The island is still there… When I try to highlight it to manipulate it, Eagle tells me that the group is empty… I also tried covering the island with brestrict… That did not help, either… Additionally, I have used a different DRC profile and I still have the same problem…
You can attach the brd file to a reply and I will see what I can do. You will have to rename the file with a .jpg extension so the forum will allow it. Then I will change it back. You can also attach the sch file so I can run a DRC check. It’s up to you.
I was able to post the Eagle files, after being approved/registered by the forum. The board files, including a couple of custom part libraries, are attached to my second post, above. They are inside the zip folder. (I have found that sites that don’t like certain files will often allow them, if they are zipped.) I have edited the file and added the schematic file, there.
I downloaded Eagle 7.2…The same problem continues. I renamed the board file in question, to break it from the schematic, ran the make-the-board function and rebuilt the board. That cleared the island in the prior location. But, now, when I run the DRC, new ghosts are appearing… When I highlight them to remove them, Eagle says, as before, that there is nothing inside the group to remove…
I really appreciate you working on this with me! Thanks!
I have removed the ground plane and redrawn it a couple of times. The offending line moves with the top line of the ground plane. This result replicates. So, here is that board file, too.
OK, I will look at that next. Couple of things. You’re are using a supply symbol for GND. All of your 5V supply is floating nets. And a ‘bullet point’ is used to denote 2 or more nets having a connection. Having a hundred bullet points just makes the schematic harder to read.
Still haven’t stated what the .pro file is for… NVM, it’s the autorouter. That’s your first problem.
Don’t know where that stray line came from. Has to be a bug in the autorouter. I am using Eagle 6.5 as I didn’t see any reason to update…
Anyway, I made a board the same as yours but manually routed it. Needless to say, it doesn’t have any errors… Added ‘v2’ to the name as to not interfere with your original.
May I asked why you are using this fab house? Seems like they don’t offer the quality as most others… Haven’t visited their site so don’t know the details… But I think 0.032 clearance and width is just awful…
codlink:
Don’t know where that stray line came from. Has to be a bug in the autorouter. I am using Eagle 6.5 as I didn’t see any reason to update…
I opened your board and ran the DRC; no ghosts... Good job! My file must just be corrupted, somehow.
Anyway, I made a board the same as yours but manually routed it. Needless to say, it doesn’t have any errors… Added ‘v2’ to the name as to not interfere with your original.
Thank you so much for going to all that trouble!
May I asked why you are using this fab house? Seems like they don’t offer the quality as most others… Haven’t visited their site so don’t know the details… But I think 0.032 clearance and width is just awful…
My selection of width and clearances was not based on the manufacturer dictates... I used wide traces and big margins to help first-time-DIYers to do the iron-on transfer method and learn to solder... I am learning what is necessary to do a production run (careful checking, Gerber files, etc.) with this project. I am using this board house, because it is so cheap. I will, likely, just share the boards.
No problem with helping, that’s what we are here for. We are just volunteers who love Sparkfun and what they stand for.
Yea, it did cross my mind that your were going the etched board route. As I understand that too thin of traces will ruin the work. If you want, once you have finalized your board, send me the files and I can look over them. Never a bad idea to have another pair of eyes to look things over. I’m pretty good at PCB design and I still make stupid mistakes that cause me to throw away the first batch from the fab house.
I just looked at the Gerbers, and a few things jump out at me:
The ground pour is very badly chopped up. Is there a particular reason you are doing this single-sided? If not, move the ground to the side without the traces. If you want to keep it single-sided. I would run the power trace around the outside of the chip and the left of the USB connector.
You really want the bypass cap grounds to have a nice path to the chip pins; ground current from C1 has to go all the way to the right side, around the power LED, and back again to get to the ground pins.
C1 and C5 should likely be 100nF ceramic caps, not electrolytics. C5 is rather well located; I would move C1 so the positive pin is closer to the IC pin
Excellent observations, Mike… Thank you for helping…
I had realized the fact that some ground signals have to go the long way around, but I am working within size limitations and there is not room for that power route. I will see if something else might work… flipping C5, adding a jumper, or some such.
Yes, this needs to be a one-sided board.
I am not the author of this circuit. C1 is before the resistor, per the instructions. I do not have enough design knowledge to know if I may move C1 to after the resistor. May I?
-C1 is electrolytic per the instructions. C5 is electrolytic, because I have it on hand. I thought that electrolytic could be used where a ceramic is specified, but not the other way around. Do I have that correctly?