Eagle Panelize PCB

ForthMonkey said:

How can i panelize PCB?

I have project with 10x5 cm PCB but i want to fit it into 10x10 cm PCB.So i will get 2 PCB from one panel but to produce this PCB they want panelized PCB. V type cutting lines but i don't know how to do it.Can someone help me for this?

Click to expand...

As Matador suggests below, instead of trying to panelize, just see what the parts cost in the quantity you require. For example, Accutrace has a deal with their boards where they charge $3/each for 10 boards up to some size (I know they do it for 10 cm by 12 cm). At order time, they ask if you want to buy more than ten, where the extras are half price (or less), and the shipping charge doesn't change.

Another option from V-scoring for separation of panelized boards is to breakaway using rat bites / mouse bites.  I was looking for a picture of that and came across this page, which seems to have some good info on design for panelization:

http://electronicdesign.com/boards/pcb-designers-need-know-these-panelization-guidelines

Exactly how you should lay out a particular panelization will depend on the design and the capabilities of the board house (what sizes of panels do they work with, what size and shape are your boards; do you have to support particular areas, allow for tooling holes, etc).

I'm still way to add V-Cut.

PCB house says "you should define a V-cut in your mechanical layer, otherwise you will receive a big boards.".

What is mechanical layer in Eagle?

ForthMonkey said:

I'm still way to add V-Cut.

PCB house says "you should define a V-cut in your mechanical layer, otherwise you will receive a big boards.".

What is mechanical layer in Eagle?

Click to expand...

If you use the draw tool, in the upper left corner (at least in my version), you can select which layer to draw - layer 100 is already called "Mechanical".  You can also choose the diameter of the tool (width of the line) while you draw.

Most important thing is to assign a unique layer when exporting the gerber. whatever layer you do it on, you can include a note with the gerber files along the lines of "layer xxx = VScore". You may also name the unique layer xxxx.vscore or something similar to make sure they see it.


Oddly enough, the method described by Bruno seems to be the only way to panellise in Eagle. Its really odd theres not a full copy feature for schematic and board.

Gustav

ForthMonkey said:

How can i panelize PCB?

I have project with 10x5 cm PCB but i want to fit it into 10x10 cm PCB.So i will get 2 PCB from one panel but to produce this PCB they want panelized PCB. V type cutting lines but i don't know how to do it.Can someone help me for this?

Thanks.

Click to expand...

Most PCB fabs would do this for you for a very low fee.
But you may want to check the Eagle forum. There are several ulp's (it's their name for "plug-ins) that will do that.

Gustav said:

ForthMonkey said:

I'm still way to add V-Cut.

PCB house says "you should define a V-cut in your mechanical layer, otherwise you will receive a big boards.".

What is mechanical layer in Eagle?

Click to expand...

If you use the draw tool, in the upper left corner (at least in my version), you can select which layer to draw - layer 100 is already called "Mechanical".  You can also choose the diameter of the tool (width of the line) while you draw.

Most important thing is to assign a unique layer when exporting the gerber. whatever layer you do it on, you can include a note with the gerber files along the lines of "layer xxx = VScore". You may also name the unique layer xxxx.vscore or something similar to make sure they see it.


Oddly enough, the method described by Bruno seems to be the only way to panellise in Eagle. Its really odd theres not a full copy feature for schematic and board.

Gustav

Click to expand...

I can't see layer 100.How can i open this one?

on eagle left menu : select : show/hide/edit layers
then select new :

if u havent done this before, layer 100 will be showing... name it, and hit ok, and hit apply...

To be honest, this sounds fraught with danger.

They haven't specified what they would like to see in this layer.  Do they want a path line for the cutting tool?  Should the path have a size?  Do they need a negative image with separators shown in-between board? What separation spacing do they need between boards?  Do they need this layer exported as a separate Gerber layer?  How would they like the layer annotated?

In all my years doing this, about the most I've ever had to do is export a separate dimension layer (layer 20 in eagle), as 99.9999% of the time your panel will be mixed with others, so having a customer define a v-score tooling path is a waste of time because you don't know what other projects will be placed on that panel.  Standard PCB panel sizes are generally around 2 ft. square, so you 10x10cm panel will be one of many that will be fabbed at the same time.

Here's the basic process of creating a panel in Eagle:
1) First off, you have to understand that Eagle doesn't like naming conflicts in the 'name' layers (layer 25 and 26).  These are the layers that the component names are drawn within.  Any entities on a panel that have the same name parameter in this layer will be re-named by Eagle when the panel is created...
2) So you first need to run "panelize.ulp" on your board.  This will copy all of the names in layer 25 to a new layer 125, where Eagle doesn't care about naming conflicts.
3) Open a brand new board *only* (don't name a schematic with the same name, or the sch -> brd consistency check will kick in), and give it a name, save it, and close it
4) Open your board, turn on all layers, then you want to select "Cut", then "Group", then select your entire design, then again select the "Cut" button, then right click on your board selection and you should see "Cut Selection" at the bottom of the list (don't ask me why such a convoluted process is required)
5) Now, close your design, and re-open your new board.  Set you grid units to whatever the board house needs between the boards.  You should be able to paste your entire board using the paste tool.  Just paste it twice to create your panel.
6) When you run your CAM job to export your Gerbers, make sure that anything that uses layer 25 (like the silkscreen layer) is switched to layer 125 (and layer 26 to 126, if you have components / names on the bottom).

When you look at your panel, you'll see Eagle has mangled layer 25 and renamed all of the components on the second (and later) copies of the board.  However the new layer 125 should have all of the original names you needed.

Hopefully that helps.

https://www.youtube.com/watch?v=avUg-devOqc

edit :
called couple of friends, some use layer 102 !!! some 20 !!!
its manufacturer depended etc etc... 
i would go with Matador's post

kambo said:

https://www.youtube.com/watch?v=avUg-devOqc

edit :
called couple of friends, some use layer 102 !!! some 20 !!!
its manufacturer depended etc etc... 
i would go with Matador's post

Click to expand...

Working at a board manufacturer, we dont care which layer was used in the design software you are using, as long as is separate and defined.

Gustav

I told mufacturer what i need.Now waiting answer.

Thanks for all helps!

Florida123 - is this spam? Please explain your relationship to ALLPCB...?

Jakob E.

"No ...."

PRR said:

"No

Click to expand...

thanx  got it...

looks like an IQ test for who knows....

JR