Panelize different board

Marco Trapanese schrieb:

I know there are ULPs to make a panel composed of identical boards.

Sometimes I need to put together different designs in order to reduce

the tooling costs.

 

Is there an easy way to do this?

I often do this. Simply use GROUP, CUT and PASTE in the board editor.

Take care to DISPLAY ALL layers before.

If the resulting combined panel consists of several boards belonging to

the same project, you can also generate the data for SMD stencil and P&P

program from it. Then the panel is assembled as a whole and separated

afterwards.

The best should be using the Gerber files.

I mean a simple program that allows you to load several boards, to place

them as you want and eventually adds the "bridges".

I fear that a "good" program able to do that is likely expensive. (The

CAM tools of the board houses can do that, but I don't know of a free or

low-cost solution to this that really works fine.)

Tilmann

Il 03/01/2013 11:17, Tilmann Reh ha scritto:

I often do this. Simply use GROUP, CUT and PASTE in the board editor.

Take care to DISPLAY ALL layers before.

But how do you put the bridges among the boards? mmm, perhaps you put

the boards very close each other so you'll ask for V-cut along the

resulting contour path.

I fear that a "good" program able to do that is likely expensive. (The

CAM tools of the board houses can do that, but I don't know of a free or

low-cost solution to this that really works fine.)

I thought it shouldn't be very expensive - the gerber files are plain

text and the software has just to translate and rotate the coordinates.

But I see the CAM tools are very expensive, indeed!

Marco

Il 03/01/2013 11:17, Tilmann Reh ha scritto:

I often do this. Simply use GROUP, CUT and PASTE in the board editor.

Take care to DISPLAY ALL layers before.

But how do you put the bridges among the boards? mmm, perhaps you put

the boards very close each other so you'll ask for V-cut along the

resulting contour path.

I fear that a "good" program able to do that is likely expensive. (The

CAM tools of the board houses can do that, but I don't know of a free or

low-cost solution to this that really works fine.)

I thought it shouldn't be very expensive - the gerber files are plain

text and the software has just to translate and rotate the coordinates.

But I see the CAM tools are very expensive, indeed!

Marco

Marco Trapanese schrieb:

Il 03/01/2013 11:17, Tilmann Reh ha scritto:

 

>> I often do this. Simply use GROUP, CUT and PASTE in the board editor.

>> Take care to DISPLAY ALL layers before.

 

But how do you put the bridges among the boards? mmm, perhaps you put

the boards very close each other so you'll ask for V-cut along the

resulting contour path.

If v-scoring is possible, I put the boards close to each other. Then I

provide separate gerber files for outline (milling) and v-score (for

which I use a custom layer in EAGLE). These files contain only extremely

thin lines (0.01 mm - not zero since this is undefined in gerber).

When I need (or want) a milled panel with bridges, I place the boards in

exactly the distance of the milling tool diameter (normally 2.0 mm,

however some board houses prefer 2.4 mm). Then I provide a separate

outline file containing all the board outlines. The board house will add

the bridges where necessary and appropriate.

If I want to explicitly define the bridge positions, I simply add WIREs

of 2.0 mm thickness to the milling layer that represent the milling

between the boards, leaving the bridges where I want them.

This has always worked with several different board houses and through

many years - without any problems, not even further inquiries by them.

>> I fear that a "good" program able to do that is likely expensive. (The

>> CAM tools of the board houses can do that, but I don't know of a free or

>> low-cost solution to this that really works fine.)

 

I thought it shouldn't be very expensive - the gerber files are plain

text and the software has just to translate and rotate the coordinates.

For a comfortable work, you also want to see what you are doing. So you

need visualisation, and prompt reaction to parameter changes. Then, you

also can't simply merge several gerber files - they will contain

different aperture definitions. Nothing that can't be dealt with, but at

least it requires some effort.

For me, putting things together within EAGLE is the best solution since

it's comfortable, available, and free - and also provides additional

benefits at manufacturing (assembly as panel, as mentioned before).

Tilmann

Il 03/01/2013 12:30, Tilmann Reh ha scritto:

If v-scoring is possible, I put the boards close to each other. Then I

provide separate gerber files for outline (milling) and v-score (for

which I use a custom layer in EAGLE). These files contain only extremely

thin lines (0.01 mm - not zero since this is undefined in gerber).

 

When I need (or want) a milled panel with bridges, I place the boards in

exactly the distance of the milling tool diameter (normally 2.0 mm,

however some board houses prefer 2.4 mm). Then I provide a separate

outline file containing all the board outlines. The board house will add

the bridges where necessary and appropriate.

 

If I want to explicitly define the bridge positions, I simply add WIREs

of 2.0 mm thickness to the milling layer that represent the milling

between the boards, leaving the bridges where I want them.

 

This has always worked with several different board houses and through

many years - without any problems, not even further inquiries by them.

I got it.

Thanks for the clear explanation.

For a comfortable work, you also want to see what you are doing. So you

need visualisation, and prompt reaction to parameter changes. Then, you

also can't simply merge several gerber files - they will contain

different aperture definitions. Nothing that can't be dealt with, but at

least it requires some effort.

I didn't say anything about the visualization because there are several

free software to view gerber files. I guess this isn't the hard part.

For me, putting things together within EAGLE is the best solution since

it's comfortable, available, and free - and also provides additional

benefits at manufacturing (assembly as panel, as mentioned before).

I agree... I will try this way.

Thanks again

Marco