Actions
Forum Thread Details
  • Replies 17 replies
  • Subscribers 173 subscribers
  • Views 3040 views
  • Users 0 members are here
Related

Custom SMD in Eagle 9.1.0

rgaillard

I have been following these guides for making a custom smd layout:

 

https://www.autodesk.com/products/eagle/blog/what-you-didnt-know-about-eagle-arbitrary-pad-shapes/

 

https://www.youtube.com/watch?v=_G0ikZKB_Ss

 

And also these guides:

 

Library Basics Part 1: https://www.autodesk.com/products/eagle/blog/library-basics-part-1-creating-first-package-autodesk-eagle/

Library Basics Part 2: https://www.autodesk.com/products/eagle/blog/library-basics-part-2-creating-first-symbol-autodesk-eagle/

Library Basics Part 3: https://www.autodesk.com/products/eagle/blog/library-basics-part-3-creating-first-device-autodesk-eagle/

 

After following these guides I placed my part on a board. However I cannot route to the custom smd pads.  I repeated the process with unmodified smds, but I still can't route to the custom library part. Based on this, I'm guessed that whatever it is that I am doing wrong is covered in the Library Basics tutorials. However, I have started fresh twice following the tutorials but I still can't get it to work. I also followed the tutorials and made the same part as in the tutorials but I can't route to the tutorial part.

 

It looks like I am not allowed to attach the library file, so I will briefly describe what I did for my custom smd (omitting some details).

 

     First, I made the footprint by placing two smds on the top layer with the smallest default size from the size drop down menu. I renamed the smds with numbers 1 and 2. Now for the custom smd, I made two arcs in the top layer. Each arc completely covered 1 smd. The arcs do not overlap each other. I then made two more sets of arcs for tstop and tcream. Finally, I made name and value placeholders in the appropriate layers. From there I made the symbol and device making sure to connect the pins and pads.

 

I have attached an image of what the part looks like when placed it on a board (there are 2 parts in this image).

 

Thanks,

Randy

 

Message was edited by: Randy Gaillard

Attachments:
image
echo_electrode_arc_1mm_200um.zip

  • Hi Randy,

     

    I see the custom pads are showing DRC errors from the Live DRC. I'm assuming you are using walkaround routing mode in which case the reason you cannot route into these pads is because in walkaround mode you cannot violate DRC, it will not let you. You need to look at why it's throwing a DRC error and fix it or change the routing mode to the non-walkaround variant to allow you to route these in manually.

     

    Best Regards,

     

    Rachael

  • in reply to rachaelp

    Thanks for the reply Rachael.

     

    I do get overlap errors, but I'm not sure what to make of that. My understanding is that Eagle should consider the custom pads to be an extension of the initially placed smds as long as the initial smds are completely covered by my custom shapes.

     

    When I use the part that I made from the Library Basics tutorials, I don't get any DRC errors, but I still can't route to the pads for that part.

     

    Thoughts?

  • in reply to rgaillard

    I'm not sure why it shouldn't be working, from what you are describing you appear to be doing it right.... If you zip your library up you should be able to attach it and then somebody will be able to take a look. If nobody has looked by the morning (it's late here now) I'll take a look in the morning image

     

    Best Regards,

     

    Rachael

  • in reply to rachaelp

    Thanks.

     

    I have uploaded a zip of the library to first post

  • in reply to rgaillard

    Hi Randy

     

    I have had  a look at your library.

    You have used a grid of 1mm and not 0.1inch when creating the symbol.

    Library symbols and the schematic need to use the 0.1 inch grid so that the net wires can connect to the pins

    The likely result of that is, if you move the device symbol in the schematic the nets will not be attached to the pins.With that being the case you will also not be seeing any air-wires to the footprint on the board and hence you cannot route to the SMD in your part.

     

    Hope this helps

    Warren

  • in reply to WarrenBrayshaw

    Thanks for the help Warren.

     

    Unfortunately, changing the grid on the symbol to 0.1 inch did not fix the problem. I re-positioned the pins on the symbol so they hit exactly at the 0.1 inch grid marks but I still can't route to the pads. I am also continuing to get DRC overlap errors.

  • in reply to rgaillard

    Are you seeing the air wires in the layout? Have you tried turning off walk around mode when routing?

     

    Best Regards,

     

    Rachael

  • in reply to rachaelp

    No I don't see any air wires and turning off walk around mode does not allow me to route to the part.

     

    I'm thinking that the problem must be with how I created the footprint but I'm at a loss as to where to start diagnosing the issue

  • in reply to rgaillard

    Hi again

     

    On the schematic, when you move the device, do the nets stay attached?

     

    Hopefully you are using the NET tool to create the nets and not the WIRE tool. The WIRE tool will get you into trouble and while similar to the NET tool the NET tool has more features to assure you get nets connected to pins

     

    I'm using  Eagle 7.7 ,After I changed the grid of the symbol editor such that the pins were on the  0.1 inch grid, I had no problems creating a schematic, adding nets and seeing airwires on the board.

    So your library is fine. A point though; you may wish to turn off the thermal tick in the package as its not useful within your custom pads.

     

    Hope this helps

    Warren

  • in reply to WarrenBrayshaw

    Ok this helps a lot.

     

    Its been several years since I have made a PCB and even longer since I've made a custom pad. I didn't remember that I needed to create a schematic before I made a board. Making a schematic first allows me to route to the parts on the board.

     

    I unchecked thermals under properties for both pads. Does turning of the thermals for the smds in the footprint change anything visually? Why do you suggest turning them off?

     

    I'm still getting DRC overlap errors. Any idea how to fix that and if overlap errors would cause a problem if I wanted to have the board made?

     

    Also, I added a tRestrict arc to both pads hoping that would prevent routing through the pad. tStop is already there. As you can see in the image the N$2 trace is going through the pad for N$1. Is there anything I can do to prevent this?

     

    image

     

    Thanks for all the help everyone