what is the way to panelize different boards using V-score(or Mouse bites)?

[Anonymous]

Hi,

now I have 3 different board, so I should make a panel for this.

1. first I import 3 boards into one new board.

2. then run panelize ulp for tName and tValue.

3. and after that draw guide rail in dimension layer and put some fiducials, tooling holes.

4. then I draw lines in V-score Layer

but after that when I turn on Manufacture Preview. It looks really weird.

certainly something is wrong..

what is the correct method for this? 

I search in google for this. but there are no information in public.

I saw a video using Gerber Tools 

but It does not match for me. because it changes all oval shape mounting holes into drill holes..

Please anyone help me out

I really need this.

Thank you

[Anonymous]

I did it myself, searching all of documents.

I hope someone could be helped.

step by step

(* [20] means dimension layer number 20 )

1. make new project and new brd

2. [20] draw guide rails (I drew it 5mm) and put some fiducials, tooling holes(3mm))

3. import my brd designs (I use 4 different board) then align it, distance between boards is 2mm

4. [20] draw breakaway tab , in my case I use Mouse-bites method. and hole size for mouse bites is 0.5mm Gap is 1mm, and draw line for connection to each board (curve is 100)

5. after all of these are conneted, I delete some of board outlines which are cross line between breakaway tab and board. (this is important, because you must make only single outline(dimension) for PCB Array)

6.  go to   Tools > Panelize..  / or use Panelize. ulp  then it will make new layers for tNames[125] and tValues[126] 

7.  then copy your whole board, then paste it.

8. almost done, you can make Cam data for your manufacturer then it's done.

I hope someday Eagle make this feature for different boards or single board to make PCB Array in effective and easy way.

[pmark23 · Accepted solution]

I save each individual PCB/Schematic as a Design Block, then in a new document import each Design Blocks to a separate Sheet and place the PCB where it should go on the PCB. Then add all the fiducials, mousebites/v-scores, etc.

The key is to have the Layer 20 outline be continuously connected -- which can be hard because the ends may look like they're connected but they're not.

It's still a pain, but much better than it used to be. Hopefully this will be made easier in the future. Updateable Design Blocks would be a huge improvement.

[Anonymous]

Yes, connecting each dimension lines for making contour is somewhat painful work.

I hope it will be updated in the near future.

[Anonymous]

Hei, i have the same issue, and i am stuck, it can't work for me, can u advice