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) Stopping TO-220 isolation
  • 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 Verified Answer
  • Replies 6 replies
  • Answers 1 answer
  • Subscribers 172 subscribers
  • Views 586 views
  • Users 0 members are here
  • eagle
  • pcb
  • isolation
  • to-220
  • stop
Related

Stopping TO-220 isolation

Former Member
Former Member over 10 years ago

I have a problem which is keeping me working over the holiday -the only thing keeping my board from fab. image I've "tried everything" and read every Googled forum, but can't find the problem addressed (everyone wants to insulate their TO-220, not the other way around).

 

I have a 7805 in a TO-220 and I want the bolt hole connected directly to the ground plane ("GND") on the bottom (and the top). Eagle insists on isolating it. It seems Eagle has lots of ways to keep traces apart, but no ways to insist "I WANT COPPER HERE NO MATTER WHAT". I've edited the part, but to no avail; packages only have holes, not vias. I've even tried illegal ways, such as putting a hole on a via (didn't work). I've messed with all the DRC's (usually with bad consequences), but even that didn't fix it. If I can't solve this, I can always edit the Gerbers... p.s. NEVER had this problem with Bishop Graphics and Datak...


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

    On 25/12/2014 3:51 p.m., Steve Ins wrote:

    I have a problem which is keeping me working over the holiday -the only

    thing keeping my board from fab. image I've "tried everything" and read

    every Googled forum, but can't find the problem addressed (everyone

    wants to insulate their TO-220, not the other way around).

     

    I have a 7805 in a TO-220 and I want the bolt hole connected directly to

    the ground plane ("GND") on the bottom (and the top). Eagle insists on

    isolating it. It seems Eagle has lots of ways to keep traces apart, but

    no ways to insist "I WANT COPPER HERE NO MATTER WHAT". I've edited the

    part, but to no avail; packages only have holes, not vias. I've even

    tried illegal ways, such as putting a hole on a via (didn't work). I've

    messed with all the DRC's (usually with bad consequences), but even that

    didn't fix it. If I can't solve this, I can always edit the Gerbers...

    p.s. NEVER had this problem with Bishop Graphics and Datak...

     

     

    Hi. One way to do it, assuming you do not wish to create a four pin device.

     

    Make the library package a three pin device and ignore the tab as that

    will be your copper pour on the top and bottom layer. Also on a user

    defined layer mark the position where the screw hole should be located.

    This will be the location you place a via at on the board.

     

     

    When you edit the board, route pins 1 thru 3 normally.

    Place a via at the location you marked in the package. Name the via GND.

    Place your GND polygons and then RATSNEST.

     

    It should all look as you desire. The board house will make the screw

    hole a plated through via as there is copper top and bottom.

     

    HTH

    Warren

     

     

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

    I think from Eagle 6 upwards you can use the arbitrary pad shape

    function and just add a polygon to the gnd tab. The 4 pad device should

    work, just make sure when you create the part that in the connect dialog

    you connect Pad2 and the new ground tab pad 4 to the same GND pin in the

    schematic symbol.

     

    Merry Xmas

     

     

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

    Steve Ins pisze:

    I have a problem which is keeping me working over the holiday -the only

    thing keeping my board from fab. image I've "tried everything" and read

    every Googled forum, but can't find the problem addressed (everyone

    wants to insulate their TO-220, not the other way around).

     

    I have a 7805 in a TO-220 and I want the bolt hole connected directly to

    the ground plane ("GND") on the bottom (and the top). Eagle insists on

    isolating it. It seems Eagle has lots of ways to keep traces apart, but

    no ways to insist "I WANT COPPER HERE NO MATTER WHAT". I've edited the

    part, but to no avail; packages only have holes, not vias. I've even

    tried illegal ways, such as putting a hole on a via (didn't work). I've

    messed with all the DRC's (usually with bad consequences), but even that

    didn't fix it. If I can't solve this, I can always edit the Gerbers...

    p.s. NEVER had this problem with Bishop Graphics and Datak...

     

    The easiest way is to put manually few GND wires over the mounting hole.

    And accept few DRC errors.

     

    Eagle avoids any copper around holes and other elements with lines in

    dimension layer - the program sets a "gap" with "clearance" width.

     

    This is very known feature (IMHO a bug) Eagle uses dimension as a

    conductive element until you set distance copper-dimension to zero. But

    in this case you have to set proper isolate of the polygon.

     

    HTH

    --

    Grzegorz Zalot

     

    complex ltd.

    office tel/fax : +48 32 2505840

    mobil : +48 501 301515

     

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

    Warren: I figure I could do it by making it 4-terminal, but that just seems so... yuk. Unfortunately, I could not get your method to work. On the board I am only allowed to place vias on layer "1-16", not on user-defined layers. At the package level, I cannot even create vias. Was this user-defined layer (i.e. layer 200) to be done at the package or board level? I tried placing a via directly under the bolt hole, but that overrode the bolt size and made the bolt hole the via diamater.

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

    Merry Xmas: It works, but it does make my library device specific to this PC board since it depends on how I routed around the pins, since the polygon must enclose the GND pin. It also gives "Package ... contains an invalid polygon." whenever I ratsnest.

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

    Grzegorz: It worked! When I tried this before, it didn't. Now I know why: The wire MUST start at or end at a GND via, not just cross over, not just connect to the GND plane, not go to a non-GND via. ALSO it must NOT start or end at the bolt center or you will get the dreaded "Can't backannotate this operation. Please do this in the schematic!" This doesn't require messing with design rules or packages. As far as a few DRC violations, Damn the torpedos!

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