Skip to main content
Topic: 1st DirtyPCB: Q about Panelization (Read 6039 times) previous topic - next topic

1st DirtyPCB: Q about Panelization

Hi - I've been hand-wiring boards for years but finally gonna try my first board here. Actually, I want to place two separate designs on the same board, then separate the boards when I receive them. That's "panelization", right?

But I'm a bit unclear on panelization. I've read some ambiguous things about it here, perhaps I'm confused because I'm not fully understanding the terms.

For a two-sided board, I've read:
Quote
Only the two layer board house allows panelizing. The PCBs must be connected by mouse bites, slots, vgroove, etc.

You cannot put multiple designs in one protopack that are not connected in some way.

So if I have two designs I want to place on one board, do I need to put an extraneous trace between them so they are "connected in some way"?

And if they are connected by a trace, why would I need to put "mouse bites, slots, vgroove, etc." between them?

Thanks for any clarification....

Re: 1st DirtyPCB: Q about Panelization

Reply #1
You have to make sure that your two (or more) designs are mechanically connected so that they don't fall apart. It's up to you how you do that. The usual method are slots with 2mm and a tab every few centimeters so that you can seperate the boards without using any tools.
http://https://blogs.mentor.com/tom-hausherr/blog/tag/mouse-bite/

Re: 1st DirtyPCB: Q about Panelization

Reply #2
here's how i submitted it and how it came out.
i did this manually in eagle by editing the dimension layer.

[attachment=0]
[attachment=1]
[attachment=2]

Re: 1st DirtyPCB: Q about Panelization

Reply #3
Thanks for the replies. The url is also helpful.

[quote author="eauth"]You have to make sure that your two (or more) designs are mechanically connected so that they don't fall apart. It's up to you how you do that. The usual method are slots with 2mm and a tab every few centimeters so that you can seperate the boards without using any tools.
[/quote]

Ahh, so my mistake is that I thought, "You cannot put multiple designs in one protopack that are not connected in some way" to mean connected electrically, instead of mechanically. Doh. Thanks for clarifying.

So with that in mind, I can place two completely independent designs on the same board, with slots and/or mouse-bites in between to facilitate separation upon receipt...have I got that correct?

...james

Re: 1st DirtyPCB: Q about Panelization

Reply #4
Yes, you got it.

 

Re: 1st DirtyPCB: Q about Panelization

Reply #5
OK, I've created a panelized Gerber file. Everything appears ok, except:

I'm not sure how to create slots/mouse bites.

I referenced the url given above and drew a set of slots and drill holes as described. The drill holes come through ok on the drill layer. But I'm not sure how to create the tab or cutout and have it properly fabricated.

I'm using Proteus/Ares. For a tab/slot, I drew a 2D rectangle with 2D circles at the ends and put it on the MECH1 layer. But I'm not sure how the fab house will handle that -- does it recognize that it's intended to be routed out?

I uploaded the Gerbers to the OSHPark site for viewing, and here's how the Board Outline looks (from "Mechanical 1.gko"):



I'd appreciate some guidance about how to confidently create a slot or mouse bite in the Gerber files...either Proteus/Ares-specific, or in general terms so I could try to get it done in the Proteus Gerber Viewer...

Thanks again for the help so far...

Re: 1st DirtyPCB: Q about Panelization

Reply #6
If you are using Eagle, you can draw that in the Dimension layer with a line width of 0.
Split up the board outline, and place arcs on the ends like shown in the picture. If you want to make it breakable, make a couple of holes. Do **not** draw a seperate outline around your boards. I can't tell you about Proteus/Ares, but a think it can be done in a rather similar way.

[attachment=0]

Re: 1st DirtyPCB: Q about Panelization

Reply #7
[quote author="eauth"]Do **not** draw a seperate outline around your boards. I can't tell you about Proteus/Ares, but a think it can be done in a rather similar way.[/quote]

OK thanks, I think I'm beginning to understand.

I'll remove the individual borders around the separate panels, and just have one around the whole board. Then, for slots or cutouts, is that just a graphic drawn on the mechanical layer? No additional information needed in the Gerber files besides a graphic of the cutout on the mechanical layer, the same layer that holds the board outline?

I'm testing my Gerbers on various online Gerber viewers and just need to know what a valid cutout should look like and on which layer.

Thanks...I'm getting closer, I think....

Re: 1st DirtyPCB: Q about Panelization

Reply #8
Quote
Then, for slots or cutouts, is that just a graphic drawn on the mechanical layer? No additional information needed in the Gerber files besides a graphic of the cutout on the mechanical layer, the same layer that holds the board outline?
Yes, that's all, just like shown in the image of my previous posting. It goes into the same layer as the board outline (.GML). Many board houses want the board outline to be included in all other layers too, although that's not strictly necessary.

Re: 1st DirtyPCB: Q about Panelization

Reply #9
[quote author="eauth"]Yes, that's all, just like shown in the image of my previous posting. It goes into the same layer as the board outline (.GML). Many board houses want the board outline to be included in all other layers too, although that's not strictly necessary.[/quote]

Thanks so much. There's a lot of conflicting info out there and I kept getting the feeling that I was missing something. Many of the available explanations are app-specific...I couldn't always relate those explanations to the Proteus/Ares app. Your explanation helped me fix the little things that were confusing me.

I just made the changes you suggested and finally my board shows actual slots when rendered on ZofzPCB:



Slowly I'm seeing how this works...just want to get it as right as possible before sending in an order...

For Proteus users: I put the outer board outline and slot graphics in the MECH1 layer within Proteus/Ares, and exported that layer instead of the BOARD EDGE layer, as Proteus calls it.

Thanks again...

Re: 1st DirtyPCB: Q about Panelization

Reply #10
[quote author="quix"]here's how i submitted it and how it came out.
i did this manually in eagle by editing the dimension layer.

[attachment=0]
[attachment=1]
[attachment=2][/quote]

Nice design! I would use more mousebites though

Re: 1st DirtyPCB: Q about Panelization

Reply #11
[quote author="Sjaak"]
Nice design! I would use more mousebites though[/quote]

Looks like a perfect PCB house capability/torture test to me, glad they passed!

Re: 1st DirtyPCB: Q about Panelization

Reply #12
Quote
[quote author="quix"]here's how i submitted it and how it came out.
i did this manually in eagle by editing the dimension layer.

[attachment=0]
[attachment=1]
[attachment=2]
[/quote]

Hey quix,

Would it be possible for you to post the gerbers (essentially the archive that you uploaded to the fab) for the PCB you showed? As you said there are software-dependent issues but if I can see what gerbers you sent out, I can generate similar ones.

Edit: not just quix, but can anyone who has successfully gotten panelized 2-layer boards from dirtypcbs please share their gerber archive sent to the fab.

Thanks!

Re: 1st DirtyPCB: Q about Panelization

Reply #13
I've used a tool by thisisnotrocketscience.nl several times now and it seems to work just fine.
The link is here: http://blog.thisisnotrocketscience.nl/p ... izer-beta/
However it is password protected (still a beta), so you might want to reach out to him on Twitter or something to get access.

In the tool you define the maximum available size (so for DirtyPCBs this will probably be 5x5cm or 10x10cm).
Then you import the gerbers of the different projects you want to include.
After that you can either manually/automatically place the boards on the available area and manually/automatically add the break tabs.
The result is a new Gerber you can sent to your PCB manufacturer.

Also, DirtyPCBs is currently the only Chinese PCB supplier I know of that allows you to do this without the boards having an electric connection.
Lots of other suppliers charge you a huge fee because you have panelized your boards if you do not do this (and even if you do, they still might end up charging you additional costs).