PADSPCB and multiple boards on same panel

[radu]

Hi all
I have 3 different .pcb files that i wanna pack up and gerber for a single panel. Has anybody done this before? i appreciate the help
radu

 

[majnoon]

One way to do it is generating Gerbers for each board and draw a panel in any Mechanical Cad tool. And send this drawing of panel with Gerbers to manufacturer.

Hope this helps.

 

[Beepster]

You put text over the part referance numbers on silk layer to save the correct part id.
Put line on silk layer over board outline.
In filter select PART,Vias,pin-pairs,text,shapes. Not-board outline.
Set grid to 1mm or 50Mils.
Select (drag box over entire board).
It is sometimes hard to get it to select all routes.
Copy (CNTRL-C)
Open next board, enter ECO mode, Paste (CNTRL-V)
In CAM, silk, don't include (Ref. Des) do inclued text on silk layer.

I do this all the time.
Good luck

 

[radu]

majnoon : i prefer to use pads and create a single gerber....it's safer; thanks though
Beepster :
What i forgot to mention probably the most important feat. is that my boards all have mixed gnd/power planes with power=7 different plane areas and 2 different grounds, the planes do not copy and also although my Preferences are set to Save all Plane Data to PCB file, when i re-open the file, my planes are not hatched anymore and i have to re-connect them.

 

[Beepster]

The planes will copy. Preferences, Drafting tab, Pour Outline. then you can select.

Planes always need re-pour after re-open file.

 

[gometric]

Agood way to do it and really easy is using CAM350. Just gerber out all the boards from powerpcb and the merge them into one file in CAM350, then gerber out again.

Gometric

 

[juggernaut7]

I agree with Gometric. Initially, in cam350 you will have a set of gerbers for each board, all in the same area. Move and align the gerber files for each board so they are in a different area and then copy the file information from two board gerbers to the first gerber. Save this file and send it out for fab. Make sure to do this for the drill files as well. The only problem you may have is if each board was done with a different set of apertures and a different tool set for the drill file. If this is the case, you will need to change the dcodes of the 2nd and 3rd file to match the first file before merging them together into the first file.

 

[yayawoo]

I totally agree. Using CAM350 is the only safe, straight forward, less chance to make error way to merge multiple pcb files into one Gerber. I did that all the time and just put break-aways between boards. They all turned out great.

 

[gometric]

Thanks guys, what I want to add is you might want to have every gerber layers and drill files from the board that you get inside cam350 aligned, that way is easier to work with the files.

Gometric

 

[kevinj]

Beepster, you're right.

But I just needed to enter ECO mode and copied and pasted without the board outline. I didn't need to :

You put text over the part referance numbers on silk layer to save the correct part id.
Put line on silk layer over board outline.
In filter select PART,Vias,pin-pairs,text,shapes. Not-board outline

Thanks a lot.

 

[Rame]

HI,

Since you have three different Pcb's ,its good to have an idea from the fabricator himself,because he would have done plenty of panels like this earlier and its easy for him to do it in no time for which we might take more time.
Few days ago i had same problem and first thing i did was to send the three gerbers to him and he helped me out to get a best panel which i wouln't have done.For your guideline please refer the underneath link,it may help you to go further.Hope this will help a bit on your above said process.

**broken link removed**


Regards

Ramesh