element14 Community
element14 Community
    Register Log In
  • Site
  • Search
  • Log In Register
  • Members
    Members
    • Achievement Levels
    • Benefits of Membership
    • Feedback and Support
    • Members Area
    • Personal Blogs
    • What's New on element14
  • Learn
    Learn
    • eBooks
    • Learning Center
    • Learning Groups
    • STEM Academy
    • Webinars, Training and Events
  • Technologies
    Technologies
    • 3D Printing
    • Experts & Guidance
    • FPGA
    • Industrial Automation
    • Internet of Things
    • Power & Energy
    • Sensors
    • Technology Groups
  • Challenges & Projects
    Challenges & Projects
    • Arduino Projects
    • Design Challenges
    • element14 presents
    • Project14
    • Project Groups
    • Raspberry Pi Projects
  • Products
    Products
    • Arduino
    • Avnet Boards Community
    • Dev Tools
    • Manufacturers
    • Product Groups
    • Raspberry Pi
    • RoadTests & Reviews
  • Store
    Store
    • Visit Your Store
    • Or 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
Autodesk EAGLE
  • Products
  • More
Autodesk EAGLE
EAGLE User Support (English) Two questions; auto router and vias
  • Blog
  • Forum
  • Documents
  • Events
  • Polls
  • Files
  • Members
  • Mentions
  • Sub-Groups
  • Tags
  • More
  • Cancel
  • New
Autodesk EAGLE requires membership for participation - click to join
Actions
  • Share
  • More
  • Cancel
Forum Thread Details
  • State Verified Answer
  • Replies 9 replies
  • Answers 2 answers
  • Subscribers 146 subscribers
  • Views 201 views
  • Users 0 members are here
Related

Two questions; auto router and vias

Former Member
Former Member over 9 years ago

I have two questions:

 

1. Some components like terminal blocks and large electrolyte capacitors are supposed to be placed directly on the PCB which means that the pins must be soldered on the bottom layer. When I use the auto router feature, it makes traces both in the top and the bottom layer. Is there a way to tell the auto router feature that all connections to specific components have to be routed in the bottom layer? (What I did as a work around: Draw a rectangle/circle in the packages top-layer to define the size of the component, ran the auto router feature and then removed the temporary rectangles/circles.)

 

2. When I make VIAs on the board, the DRC gives a clearance error because the top and bottom traces overlap in the VIA-point. This happens even if the VIA is identical to those made by the auto router feature (which don't cause clearance error). What am I doing wrong?

 

Thanks for any help!

  • Sign in to reply
  • Cancel
  • autodeskguest
    0 autodeskguest over 9 years ago

    Am 09.06.2014 18:35, schrieb Olav S. Flaa:

    I have two questions:

     

    1. Some components like terminal blocks and large electrolyte capacitors

    are supposed to be placed directly on the PCB which means that the pins

    must be soldered on the bottom layer. When I use the auto router

    feature, it makes traces both in the top and the bottom layer. Is there

    a way to tell the auto router feature that all connections to specific

    components have to be routed in the bottom layer? (What I did as a work

    around: Draw a rectangle/circle in the packages top-layer to define the

    size of the component, ran the auto router feature and then removed the

    temporary rectangles/circles.)

     

    2. When I make VIAs on the board, the DRC gives a clearance error

    because the top and bottom traces overlap in the VIA-point. This happens

    even if the VIA is identical to those made by the auto router feature

    (which don't cause clearance error). What am I doing wrong?

     

    Thanks for any help!

     

    --

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

    http://www.element14.com/community/message/115764

     

     

    1. Autorouter/General-Tab setting N/A into a layer will block the use.

    2. Can't say directly but something does not fit the design rules.

     

    --

    Mit freundlichen Grüßen / With best regards

     

    Joern Paschedag

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • Former Member
    0 Former Member over 9 years ago in reply to autodeskguest

    Thanks for your reply!

     

    Unfortunately I can't block the top layer, I need to auto route using both the bottom and top layer. But the routing to/from a few specific components has to be on the bottom layer.

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • Former Member
    0 Former Member over 9 years ago

    1. It would be nice if someone could confirm that this isn't possible if that is the case.

    2. This is still a mysterium to me. But I will hopefully figure it out sometime.


    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 9 years ago in reply to Former Member

    Am 14.06.2014 09:57, schrieb Olav S. Flaa:

    1. It would be nice if someone could confirm that this isn't possible if

    that is the case.

    2. This is still a mysterium to me. But I will hopefully figure it out

    sometime.

     

     

     

    --

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

    http://www.element14.com/community/message/116687

     

     

    Place an area "trestrict" around parts you don't want to connect on top.

    Help layer.

     

    --

    Mit freundlichen Grüßen / With best regards

     

    Joern Paschedag

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Reject Answer
    • Cancel
  • Former Member
    0 Former Member over 9 years ago in reply to autodeskguest

    1. Thank you! This is exactly what I needed.

    2. I have found what the problem was. I inserted a via and connected one trace from the top layer and another from the bottom layer, both connected to the same net. But the via didn't automatically switch to that net, but was connected to its own separate net. So I had to manually give the vias the same net name as the traces connected to them. I didn't know that a via had its own net. And I don't understand why there was no question similar to when I connect two wires in the schematics view, but I assume there is a reason for it that I'm not capable to understand yet.

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 9 years ago in reply to Former Member

    On 14/06/14 16:25, Olav S. Flaa wrote:

    I didn't know that a via had its own net. And I don't understand

    why there was no question similar to when I connect two wires in the

    schematics view, but I assume there is a reason for it that I'm not

    capable to understand yet.

     

    I suppose I can see how this is confusing, but it does make sense.

     

    First off, understand the purpose of the two editors:

       The schematic editor is used to draw a representation (schematic) of

    the function of the circuit. It defines what the circuit is, including

    which pins are connected to which others.

       The board editor is used to lay out the physical components and

    copper in such a way as to achieve the circuit defined by the schematic.

     

    Now, a consequence of this is that any change to the circuit must be

    done on the schematic, not the board. If you connect two nets together

    on the schematic, that's considered a change to the circuit and you are

    asked how to resolve the change. If you connect two nets together on the

    board, that's an error, which will be flagged up by DRC.

     

    So what if you add a via on the board? There could be two reasons - you

    might want to run a net through it or you may just be making a hole for

    mounting purposes. In both cases there are better ways to do this, but

    the important thing is that Eagle doesn't know which you intended.

    Either way, the via has a net associated with it as part of its nature,

    but the editor doesn't know which net you intended until you rename it.

    So it creates it with a newly allocated, unique net all of its own. That

    may not even be wrong, in fact.

     

    Hope that helps,

    Rob

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • Former Member
    0 Former Member over 9 years ago in reply to autodeskguest

    Thanks for your helpful explaination!

    I thought vias were for connecting nets through holes and holes/drills was for making holes for mounting purposes (I read in the help-file that drills are conducting through holes but holes are not). Although I know the purpose of the schematic versus the board and that any changes in the circuits have to be done in the schematic, I didn't realize that this of course has to be the consequence of it:

    "If you connect two nets together on the schematic, that's considered a change to the circuit and you are asked how to resolve the change. If you connect two nets together on the board, that's an error, which will be flagged up by DRC."

    In addition I didn't know this:

    "via has a net associated with it as part of its nature, but the editor doesn't know which net you intended until you rename it. So it creates it with a newly allocated, unique net all of its own."

    But now I know :-)

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 9 years ago in reply to Former Member

    Olav S. Flaa wrote:

    I thought vias were for connecting nets through holes and holes/drills

    was for making holes for mounting purposes (I read in the help-file that

    drills are conducting through holes but holes are not). Although I know

    the purpose of the schematic versus the board and that any changes in

    the circuits have to be done in the schematic, I didn't realize that

    this of course has to be the consequence of it:

    "If you connect two nets together on the schematic, that's considered a

    change to the circuit and you are asked how to resolve the change. If

    you connect two nets together on the board, that's an error, which will

    be flagged up by DRC."

    In addition I didn't know this:

    "via has a net associated with it as part of its nature, but the editor

    doesn't know which net you intended until you rename it. So it creates

    it with a newly allocated, unique net all of its own."

     

    Placing vias by hand is normally not neccessary.

     

    Vias will be created automatically, in the course of routing an

    airwire, whenever you change the layer (middle mouse button or

    dropdown layerlist in the tool bar).

     

    Vias will also be generated when you change the layer of a track.

     

    Should it be neccessary to create vias be hand - for instance to tie

    GND planes in different layers together, you can use the via command

    with the net name as parameter like: "via 'GND".

    --

     

    Lorenz

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • Former Member
    0 Former Member over 9 years ago in reply to autodeskguest

    Aha, very useful information, thank's a lot!

    It takes A LOT of time to learn complex software like this. Some programs take years to master, I assume Eagle is one of those. Luckily, I only need it for fairly simple audio-circuits.

    • 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 © 2023 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