Actions
Forum Thread Details
  • Replies 16 replies
  • Subscribers 182 subscribers
  • Views 2138 views
  • Users 0 members are here
Related

Need devices with multiple packages

Former Member

My company has designed boards in EAGLE for years, and it's worked well for us.  However, this year, we had a problem with EAGLE and a composite part that caused a run of boards to be populated incorrectly.  Cadsoft support suggested we post a feature request here to resolve this issue and help us avoid rework costs in the future.

 

ISSUE:

We noticed the issue when a board we designed came back from the manufacturer with all parts populated except for two 50-pin header sockets.  Looking further, we noticed that while these parts had a footprint in the layout, they were not listed in the BOM, which we had taken directly from EAGLE.  Their absence from EAGLEs BOM had to do with a mechanical constraint that we needed to place on them.

 

EXPLANATION:

Now these two 50-pin header sockets, J1 and J2, needed to be precisely spaced in order to seat a daughterboard with mating connectors.  Our board designer, a Mechanical Engineer, noticed after precisely placing J1 and J2 that one of them could be moved anywhere in the layout, destroying their mechanical compatibility with the daughter board.  In order to constrain them to the proper spacing and ensure that they'd always move as a pair, he created a custom device in our library with both of their footprints properly aligned and spaced.  Now the daughterboard's mechanical interface cannot be broken by an inadvertent drag-and-drop or by the autorouter.

 

The only trouble with this custom part, however, is that EAGLE does not support composite devices (a device that is placed like one package on the layout, but is really two devices on the BOM) and therefore our custom part could not correctly update the BOM.  However, EAGLE could resolve this by supporting one of both of the following features:

 

RESOLUTION:

Support for composite devices in libraries.  This would be comprised of any two or more library devices on the schematic -- and their packages on the layout -- with the packages being physically constrained to a fixed spacing.

 

Another solution would be if we could group individual packages on the layout so that when any package in the group was moved (via drag-and-drop or the auto-router) the other packages would move with it.  The important part here is that the packages don't need to be locked to the board--they just need to be locked in relative position to the other packages in a group.

 

Both of these solutions would keep EAGLEs BOM accurate without permitting a violation of any mechanical specifications.

 

Thanks for your time!  We look forward to seeing future improvements to EAGLE!

Parents

  • I also need this functionality. I am placing a DART SoC module which connects to the main board via two headers. I would like to treat the module as one component in the schematics, and place it, move it, etc in layout as one component, but build it of two devices in the library.

     

    I think a good solution would to have packages work the same way a symbol in the device editor: you can add multiple symbols to a device and draw on the "composite symbol" in an editor looking like the schematics editor. It should be possible to edit the package the same way, where you could add multiple packages and edit it in an editor looking like the layout editor.

     

    Using daughter board modules is a very common ting, so I recon this feature will be helpful for many users.

  • in reply to maxq

    On 25.05.2016 13:46, Marius Aabel wrote:

    I also need this functionality. I am placing a DART SoC module which

    connects to the main board via two headers. I would like to treat the

    module as one component in the schematics, and place it, move it, etc in

    layout as one component, but build it of two devices in the library.

     

    I think a good solution would to have packages work the same way a

    symbol in the device editor: you can add multiple symbols to a device

    and draw on the "composite symbol" in an editor looking like the

    schematics editor. It should be possible to edit the package the same

    way, where you could add multiple packages and edit it in an editor

    looking like the layout editor.

     

    Using daughter board modules is a very common ting, so I recon this

    feature will be helpful for many users.

     

    I think you are trying to solve a common problem the hard way. Try this:

    -Copy the single plug package, paste it twice on a new package.

    -Named the new package it after the soc board, not the plug!

    -Draw placement drawings of the full board outline at tPlace.

    -Add mounting holes too with correct relative placement.

    -If there are space limitations between the soc and your pcb, put that

    very visible on the package too.

    -Make sure the valuable relative placement is correct. It may be lost

    the way you describe.

    -Give the two instances different logical pin names that match what the

    soc is using, like U1-1,U1-2,....U2-1,U2-2.. for example. Remember the

    pin number doesnt have to be a numeric. Strings will do.

     

    Ive done this with success on comExpress modules and I can't understand

    why you want to do it a different way. Its after all the SOC you are

    describing, and not the single plug. This is not hard to do.

     

  • in reply to autodeskguest

    CadSoft Guest wrote:

     

    Ive done this with success on comExpress modules and I can't understand

    why you want to do it a different way. Its after all the SOC you are

    describing, and not the single plug. This is not hard to do.

     

     

    When the board is sent to manufacturing, the pick and place is not going to mount one single component, but two header plugs. For the PCB manufacturer, this is not one component, it is two. The BOM would have to be manually edited instead of using automatic integrations to Eagle.

     

    So, what I am probably going to do, is make the module into two components, each with one header. It is more important for me to keep the PCB correct, than the schematic.

Reply
  • in reply to autodeskguest

    CadSoft Guest wrote:

     

    Ive done this with success on comExpress modules and I can't understand

    why you want to do it a different way. Its after all the SOC you are

    describing, and not the single plug. This is not hard to do.

     

     

    When the board is sent to manufacturing, the pick and place is not going to mount one single component, but two header plugs. For the PCB manufacturer, this is not one component, it is two. The BOM would have to be manually edited instead of using automatic integrations to Eagle.

     

    So, what I am probably going to do, is make the module into two components, each with one header. It is more important for me to keep the PCB correct, than the schematic.

Children
  • in reply to maxq

    Marius Aabel schrieb:

     

    When the board is sent to manufacturing, the pick and place is not going

    to mount one single component, but two header plugs. For the PCB

    manufacturer, this is not one component, it is two. The BOM would have

    to be manually edited instead of using automatic integrations to Eagle.

     

    So, what I am probably going to do, is make the module into two

    components, each with one header. It is more important for me to keep

    the PCB correct, than the schematic.

     

    However, take care that with your method you get the maximum chance to

    make your board completely invalid, by putting the two connectors (and

    eventually additional mechanical things like centering or mounting

    holes) in the wrong relation to each other.

     

    For me, it is also most important to keep the PCB correct, and that's

    exactly why I use a single package in such cases.

     

    Manually editing the BOM for P&P appears as the much better way to go...

     

    Tilmann

     

  • in reply to autodeskguest

    Manually editing the BOM for P&P appears as the much better way to go...

     

    Tilmann

     

    Thanks! Valuable tips!

  • in reply to autodeskguest

    On 25.05.2016 14:57, Tilmann Reh wrote:

    Marius Aabel schrieb:

     

    When the board is sent to manufacturing, the pick and place is not going

    to mount one single component, but two header plugs. For the PCB

    manufacturer, this is not one component, it is two. The BOM would have

    to be manually edited instead of using automatic integrations to Eagle.

     

    So, what I am probably going to do, is make the module into two

    components, each with one header. It is more important for me to keep

    the PCB correct, than the schematic.

     

    However, take care that with your method you get the maximum chance to

    make your board completely invalid, by putting the two connectors (and

    eventually additional mechanical things like centering or mounting

    holes) in the wrong relation to each other.

     

    For me, it is also most important to keep the PCB correct, and that's

    exactly why I use a single package in such cases.

     

    Manually editing the BOM for P&P appears as the much better way to go...

     

    We could also ask the rhetoric question:

     

    Whats best for your project between:

     

    1-The manufacturers finds an issue with pick and place files that doesnt

    seem to match the board, and contacts you about this.

     

    vs

     

    2-You find that your soc doesnt fit after the board is manufactured.

     

     

  • in reply to autodeskguest

    Morten Leikvoll schrieb:

     

    We could also ask the rhetoric question:

     

    Whats best for your project between:

     

    1-The manufacturers finds an issue with pick and place files that doesnt

    seem to match the board, and contacts you about this.

     

    vs

     

    2-You find that your soc doesnt fit after the board is manufactured.

     

    That's exactly the point here.

     

    Tilmann

     

  • in reply to autodeskguest

    I have to ask, why did the boards actually come back without the parts

    fitted? Any good CM would have contacted you with a query which you would

    have answered and your board would have been correctly populated. I suggest

    you should think long and hard about if your current CM is giving you an

    adequate service....

     

    On my BOM's I list ALL part and have them marked as fitted or not fitted so

    there is no doubt as to my intentions. Then any pads on the board that

    don't have a corresponding line in the BOM, whether fitted or not are an

    issue that needs to be addressed.

     

    For me, all my parts have a unique in house part number which then maps to

    either a manufacturers part number or a sub-BOM so if there was a case

    where I needed to create a composite component it would have a unique part

    number which would call up it's own sub-BOM with all the parts it

    contained. My system, once finished will roll these parts into the main BOM

    automatically.

     

    Best Regards,

     

    Rachael

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

  • in reply to autodeskguest

    I have to ask, why did the boards actually come back without the parts

    fitted? Any good CM would have contacted you with a query which you would

    have answered and your board would have been correctly populated. I suggest

    you should think long and hard about if your current CM is giving you an

    adequate service....

     

    On my BOM's I list ALL part and have them marked as fitted or not fitted so

    there is no doubt as to my intentions. Then any pads on the board that

    don't have a corresponding line in the BOM, whether fitted or not are an

    issue that needs to be addressed.

     

    For me, all my parts have a unique in house part number which then maps to

    either a manufacturers part number or a sub-BOM so if there was a case

    where I needed to create a composite component it would have a unique part

    number which would call up it's own sub-BOM with all the parts it

    contained. My system, once finished will roll these parts into the main BOM

    automatically.

     

    Best Regards,

     

    Rachael

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

  • in reply to autodeskguest

    I have to ask, why did the boards actually come back without the parts

    fitted? Any good CM would have contacted you with a query which you would

    have answered and your board would have been correctly populated. I suggest

    you should think long and hard about if your current CM is giving you an

    adequate service....

     

    On my BOM's I list ALL part and have them marked as fitted or not fitted so

    there is no doubt as to my intentions. Then any pads on the board that

    don't have a corresponding line in the BOM, whether fitted or not are an

    issue that needs to be addressed.

     

    For me, all my parts have a unique in house part number which then maps to

    either a manufacturers part number or a sub-BOM so if there was a case

    where I needed to create a composite component it would have a unique part

    number which would call up it's own sub-BOM with all the parts it

    contained. My system, once finished will roll these parts into the main BOM

    automatically.

     

    Best Regards,

     

    Rachael

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.