element14 Community
element14 Community
    Register Log In
  • Site
  • Search
  • Log In Register
  • Community Hub
    Community Hub
    • What's New on element14
    • Feedback and Support
    • Benefits of Membership
    • Personal Blogs
    • Members Area
    • Achievement Levels
  • Learn
    Learn
    • Ask an Expert
    • eBooks
    • element14 presents
    • Learning Center
    • Tech Spotlight
    • STEM Academy
    • Webinars, Training and Events
    • Learning Groups
  • Technologies
    Technologies
    • 3D Printing
    • FPGA
    • Industrial Automation
    • Internet of Things
    • Power & Energy
    • Sensors
    • Technology Groups
  • Challenges & Projects
    Challenges & Projects
    • Design Challenges
    • element14 presents Projects
    • Project14
    • Arduino Projects
    • Raspberry Pi Projects
    • Project Groups
  • Products
    Products
    • Arduino
    • Avnet Boards Community
    • Dev Tools
    • Manufacturers
    • Multicomp Pro
    • Product Groups
    • Raspberry Pi
    • RoadTests & Reviews
  • Store
    Store
    • Visit Your Store
    • Choose another store...
      • Europe
      •  Austria (German)
      •  Belgium (Dutch, French)
      •  Bulgaria (Bulgarian)
      •  Czech Republic (Czech)
      •  Denmark (Danish)
      •  Estonia (Estonian)
      •  Finland (Finnish)
      •  France (French)
      •  Germany (German)
      •  Hungary (Hungarian)
      •  Ireland
      •  Israel
      •  Italy (Italian)
      •  Latvia (Latvian)
      •  
      •  Lithuania (Lithuanian)
      •  Netherlands (Dutch)
      •  Norway (Norwegian)
      •  Poland (Polish)
      •  Portugal (Portuguese)
      •  Romania (Romanian)
      •  Russia (Russian)
      •  Slovakia (Slovak)
      •  Slovenia (Slovenian)
      •  Spain (Spanish)
      •  Sweden (Swedish)
      •  Switzerland(German, French)
      •  Turkey (Turkish)
      •  United Kingdom
      • Asia Pacific
      •  Australia
      •  China
      •  Hong Kong
      •  India
      •  Korea (Korean)
      •  Malaysia
      •  New Zealand
      •  Philippines
      •  Singapore
      •  Taiwan
      •  Thailand (Thai)
      • Americas
      •  Brazil (Portuguese)
      •  Canada
      •  Mexico (Spanish)
      •  United States
      Can't find the country/region you're looking for? Visit our export site or find a local distributor.
  • Translate
  • Profile
  • Settings
Autodesk EAGLE
  • Products
  • More
Autodesk EAGLE
EAGLE User Support (English) How to apply net class to unconnected pad?
  • Blog
  • Forum
  • Documents
  • Events
  • Polls
  • Files
  • Members
  • Mentions
  • Sub-Groups
  • Tags
  • More
  • Cancel
  • New
Join Autodesk EAGLE to participate - click to join for free!
Actions
  • Share
  • More
  • Cancel
Forum Thread Details
  • State Not Answered
  • Replies 8 replies
  • Subscribers 173 subscribers
  • Views 1386 views
  • Users 0 members are here
  • pad
  • pin
  • class
  • creepage
  • net
  • unconnected
  • clearance
Related

How to apply net class to unconnected pad?

electrodevab
electrodevab over 10 years ago

Hi all,

 

I would be glad to have some input on an issue I ran into recently:

 

Assume I added a diode in a sot23 package. The diode symbol only have two (anode and cathode) connecting pins but the package has three pads. To the two connecting pins I assign netclasses with different clearance and creepage restrictions but then there will be no netclass assigned to the third pad of the package. This generates tons of errors when running drc and I dont have full control of the clearance and creepage distances.

 

For the devices I create myself I can add a connecting pin for each pad in the device and then add a short unconnected net to the unconnected pads so that I can apply a netclass. This is not the correct way to do it, does anyone know if is there any other way to do this?

 

/Tomas

  • Sign in to reply
  • Cancel
  • kikoun
    0 kikoun over 10 years ago

    Hi,

     

    I had the same trouble on some high voltage gate drivers (unconnected pin class). I don't have no other solution than your, and i would be glad if someone have a better solution...

     

    Guillaume.

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago

    On 2/02/2015 9:06 p.m., Tomas Bergh wrote:

    Hi all,

     

    I would be glad to have some input on an issue I ran into recently:

     

    Assume I added a diode in a sot23 package. The diode symbol only have

    two (anode and cathode) connecting pins but the package has three pads.

    To the two connecting pins I assign netclasses with different clearance

    and creepage restrictions but then there will be no netclass assigned to

    the third pad of the package. This generates tons of errors when running

    drc and I dont have full control of the clearance and creepage

    distances.

     

    For the devices I create myself I can add a connecting pin for each pad

    in the device and then add a short unconnected net to the unconnected

    pads so that I can apply a netclass. This is not the correct way to do

    it, does anyone know if is there any other way to do this?

     

    You say you get "tons of errors" to this unconnected pad so I assume it

    is a polygon pour that is getting too close to this unused pad. If this

    is the case keep the polygon away by surrounding the pad with a fence

    wires on the tRestrict layer.The width of the wire is at least the

    clearance you require and should be close to but not touch the pad.

     

    HTH

    Warren

     

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • electrodevab
    0 electrodevab over 10 years ago in reply to autodeskguest

    Hi,

    No, I do not use a fill in the top layer here. The clearance issues of importance are between the unconnected pad (top right pad of D9) and the other two pads on the same sot23 package. (D9)

    There are also clearance errors to other components in this example. (between T1, D7 and D9)

     

    image

     

    Any ideas?

     

    Regards,

    Tomas

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • dukepro
    0 dukepro over 10 years ago in reply to electrodevab

    Tomas,

     

    There will not be a way to do this in the schematic since the

    unconnected pin is not represented in the symbol.  I haven't found a way

    to do this in the board, either.  But I can think of a couple of

    workarounds.

     

    It may seem like going around one's elbow to get to one's hand to solve

    this, but there are ways.

     

    First method, edit the connections on the device in the library and add

    the unconnected pad to either the cathode or the anode.  Make sure the

    connection type is "all", not "any".  The pro in this method is that the

    pad assumes the same class as whatever net is connected to the

    cathod/anode.  The con to this is that it has an impact on any design

    that uses that device/package.  You'll have to route a trace from the

    otherwise unconnected pad to one of the other two, but this shouldn't

    have any impact since you won't have any unrelated traces threading

    their way through a SOT23 (or at least shouldn't).

     

    Second method would be to create a diode symbol that has an extra pin

    named "NC".  Create a device (DIODE3 perhaps?) using this symbol and the

    SOT23 package and connect appropriately.  The replace your diode in the

    schematic with the DIODE3 device.  Now you have a way to assign a class

    to the pin.  You also have a way to connect the NC pin to either the

    cathode or the anode, whichever provides easier routing.

     

    The caution in both of these methods is that you MUST be sure that the

    unconnected pad on the diode is truly not connected to anything - not

    even the substrate.

     

    A third method is probably easiest - ditch the single diode and go with

    a dual diode in a SOT23 - there might not be any price difference, and

    if so, it's probably minimal.  You can choose which of the two diodes to

    use based on ease of routing.  Whether or not a dual diode can be found

    to fit your requirements and pricing is a design decision.

     

     

    HTH,

        - Chuck

     

     

    On 02/03/2015 02:02 AM, Tomas Bergh wrote:

    Hi,

    No, I do not use a fill in the top layer here. The clearance issue of

    importance are between the unconnected pad (top right pad of D9) and the

    other two pads on the same sot23 package. (D9)

    There are also clearance errors to other components in this example.

    (between T1, D7 and D9)

     

     

     

    Any ideas?

     

    Regards,

    Tomas

     

    --

    To view any images and attachments in this post, visit:

    http://www.element14.com/community/message/139172

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • electrodevab
    0 electrodevab over 10 years ago in reply to dukepro

    Hi,

     

    Thanks for your effort Chuck and Warren. I am thankful.

     

    I think the easiest workaround is just to approve the ERC-errors and check the clearance manually...

    As the person I am I prefer it to be correct and this is the reason for asking here.. image

     

    I just leave the thread as unsolved for now and maybe someone releases some proper solutions that actually solve this issue now or later.

     

    Thanks,

    Regards

    Tomas

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • kikoun
    0 kikoun over 10 years ago in reply to dukepro

    Hi,

     

    On some special device (high voltage gate driver) I have this problem. I add a pin on the symbol for each unconnected pin. In schematic I draw a wire connected to this only pin and I set the class of this wire. I get 2 warning : One because I connect a "NC" pin, and a second because the wire is connected to only one pin....

    This solution is not perfect because you still get 2 error to approve, but it's better for controlling polygon, and easier to approve 2 warning in schematic than several in board....

     

    The perfect solution will be to let us define the class on unconnected pad in the board editor, but I guess that is for the 'suggestion forum. And IMO, this is not the most urgent, since there is a workaround.

     

    Guillaume.

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • electrodevab
    0 electrodevab over 10 years ago in reply to kikoun

    Hi Guillaume,

    Yes, this is how I did earlier and it solves the issue but I would like to get around this without having to make a special device with pins for all pads.

    Thanks,

    /Tomas

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • kikoun
    0 kikoun over 10 years ago in reply to electrodevab

    Hi Thomas,

     

    I don't have better solution, and I think that there is no better one with the today's eagle version.

    The best way would be to be able to select a pad (in board editor) and change the class, or maybe in schematic editor a way to select the class of every unconnected pin of the package.. But it's not possible (for now).

    Sorry !

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
element14 Community

element14 is the first online community specifically for engineers. Connect with your peers and get expert answers to your questions.

  • Members
  • Learn
  • Technologies
  • Challenges & Projects
  • Products
  • Store
  • About Us
  • Feedback & Support
  • FAQs
  • Terms of Use
  • Privacy Policy
  • Legal and Copyright Notices
  • Sitemap
  • Cookies

An Avnet Company © 2025 Premier Farnell Limited. All Rights Reserved.

Premier Farnell Ltd, registered in England and Wales (no 00876412), registered office: Farnell House, Forge Lane, Leeds LS12 2NE.

ICP 备案号 10220084.

Follow element14

  • X
  • Facebook
  • linkedin
  • YouTube