Paparazzi Tiny13 v1.1 PCB question

[Uttam1]

Hi Guys,

Just finished populating my 1st Tiny board. I'm a bit stumped with the PCB though. There is no common ground connection running through the servo connector pads? There is a common +ve running through them all, but no common ground! Could someone please help me?

-Thanks,
Uttam- India, Bangalore
http://www.microbrushless.com

[AntonK]

mmm, there should be. May I ask where you got your PCB from? The Common ground runs through one of the interior layers(its a 4 layer board) maybe thats why you cant "see" it?

[Uttam1]

OK, there is no mention of this on the paparazzi website! Where do I get the PCB's from?

[AntonK]

No mention of what? The fact that it is 4 layers? That is shown in the Eagle files. I was asking where you got your PCB because I know of 1 or 2 people who didnt create their gerbers correctly, and only printed a 2 layer board.

Anton

[Uttam1]

Yes, since this is for a hobbiest too, why take it for granted that he has the full blown version of Eagle? Anyway, could you e-mail a jpg of the layout? Maybe 1 each for each layer, it you have the time? That would be very helpful ( nchandrashekhar@gmail.com ). I need to know what the interconnects in the middle 2 layers are. The PCB was created using gerber's from the free version of Eagle....and we have a fully populated 2 LAYER BOARD!

Thanks in advance

[HoverMonkey]

hmm, I followed director on creating Grber files from Eagle files and it came out as a 2 layer board also.

Can you elaborate on how to see in Eagle that it is a 4 layer board?

[Uttam1]

The only way I think is to have the full blown version of Eagle ( $199 ). Anyone here with the full blown version, it'd be of immense help if you could mail the extended gerber plots for all 4 layers!

-TIA
Uttam

[AntonK]

This question has been posted on the paparazzi user group. I may be mistaken that you can create 4 layer gerbers from the free version. I do know you can see all 4 layers using the free version

[Uttam1]

Thanks Anton, your help is much appreciated! Last night, I sat with Eagle and generated the Gerbers. I did a google and found out how to generate Gerbers for multilayer PCB's using Eagles Cam processor. I used viewmate to view the Gerbers, and figured out where we went wrong. Thanks again, it was your suggestion that made me look at Eagle's layer structure and understand it! Meanwhile, another kind person on the paparazzi list mailed me the Gerbers, and they match the once I generated last night. Now, off the the PCB shop :)

If anybody here is interested and has questions on how to generate additional layers using Eagles Cam processor, remember that the Tiny is a 4 layer PCB, Top, Route2, Route15 and Bottom. For instructions on creating Gerbers for multilayer PCB's using Eagle:

1. From the EAGLE control panel click on File/Open/Board and select the board you are interested in.

2. Click on the CAM processor ICON.

3. Now click File/Open/JOB and select the file called GERBER.CAM from the CAM directory. If EAGLE prompts you to save the current process. Click NO.

4. Notice on the CAM processor screen a field called SECTION. If, the section called “Generate a wheel file” is not visible, then click on the down arrow at the end of the section and select the section called Generate a Wheel File.

5. On the right hand side of the CAM processor screen you will notice the layer list. Tag the additional layers you wish to include: Any inner layers or maybe the bottom silk screen layers (BPlace and BName). DO NOT UNTAG ANY OF THE OTHER LAYERS. Click on File/Save Job to save what we have done so far. I would recommend giving this CAM job a different name. For example, 4Layer.cam)

6. After tagging all the necessary layers click on the SECTION down arrow and select the very last section called Solder Stop Mask SOL.

7. Click on the ADD button. EAGLE will ask you to name the new section you are creating. You can give it any name you feel comfortable with, example, call it INNER POWER PLANE VCC, INNER SIGNAL LAYER 2, or BOTTOM SILK SCREEN). Click OK when done.

8. Now select the appropriate layer for this section. If its an inner power plane (for example $GND) only select that layer by itself. If it’s a bottom silk screen layer tag the Dimension, BPlace and BName layers. If it’s a regular signal layer combine it with PAD’s and VIA’s MAKE SURE NO OTHER LAYERS ARE TAGED.

9. Change the name of the output. Use the table in the bottom of this page as an example.

10. Create a new section for every new layer needed. Repeat step 7, 8, 9 and 10 for every new layer.

11. Go to step 4 on page number 1.

Instructions from:

http://72.14.235.104/search?q=cache:QKuATfzOMnkJ:www.apcircuits.com/resources/downloads/Excellon.doc+eagle+.brd+generating+gerber&hl=en&ct=clnk&cd=9

Hope this is of some help to someone!

-Uttam

[AntonK]

Awesome! Good work! I havent really had to work with it much, so I was really shooting from the hip.

Anton