Actions
Forum Thread Details
  • State Not Answered
  • Replies 4 replies
  • Subscribers 181 subscribers
  • Views 546 views
  • Users 0 members are here
Related

Flounder meets the CONNECT command (and loses)

supuflounder

I'm feeling more like Bambi in "Bambi meets Godzilla".

 

I have a symbol.  I gave the pins name like NOA, COMA, NCA (yes, it's a relay!  A genuine metal-on-metal contact set.  There are sound reasons for this, mostly dealing with forward voltage drop across MOSFETs messing up the circuit and also limiting the total current draw due to their resistance).  I spent most of the  night switching between various tutorials and Eagle.  I have pads, and the pads have names like P$2, P$3, etc.  Then I get to the Device level, and want connect something like P$4 with NOA, P$5 to COMA, and P$6 to NCA (no, I don't remember the pin mappings, and I want to go to bed...).  What I expected is what is shown in all the tutorials. What I get is a dialog with an empty pin list, as shown in the attached screenshot.  Just to show the the device has pin names (which I renamed from P$1, etc.), I show the symbol view.  But I put the pins down, then renamed them.

 

I really am a newcomer to Eagle; I've been using it less than a week, and this is my first attempt to create a part.  I feel that i understand enough about .brd and .sch to make progress, albeit more slowly than an expert, but there aren't any prebuilt libraries I could find for this part, so decided that it was time to stretch my understanding and build my own part.

 

I am using 9.1.1, which was current when I started last week; 9.1.2 is now out, but I have not yet upgraded.

 

The tutorials I've found are clear, but they all end up with a set of pins to be connected to a set of pads.  I have no set of pins, and do not understand why. I would appreciate if someone could point out what I've done wrong and/or tell me how to fix it.

 

Also, the only file I found was a .lbr file; I presume it contains both the .sch and .brd components magically within itself.  And when I add it, it includes the file with the #1 in its name.  I am too tired to worry about that right now. [If it does not appear, it is because I got an error message about "The content type of this file" not being a permitted attachment.  Typical sloppy work; a real message would have given the file name, since I had four attachments.  Or, it would have highlighted the forbidden attachment.].

 

      joe

(aka "The Supuflourous Flounder)

Attachments:
image
image
Parents
  • 0

    Hello

    I believe you have not followed the library creation tutorials properly.

     

    It's  three step process.

    Create a package

    Create the symbols that will be used in the device

    Create a device using a previously created package and the previously created symbols.

    Only then will the "connect" dialog show pins of the device and pads of the Package (footprint)

     

    Have a look at one of the Eagle supplied libraries for a relay. (relay.lbr)

    Open relay.lbr

    Display the Device RT42?*

    You will see the Device is composed of three symbols and a package (footprint)

    Using the Information tool (I) you will see the names of the Symbols are "K" and "U".

    The symbol "U" has been used here twice.

    Each symbol placed into the Device is referred to as a "Gate"

    Using the Information tool (I) you will see the names of the gates are "1" "2" and "3"

     

    The pin numbers displayed in the device editor only appear after the "connect" is made. Prior to that they appear in the "connect" dialog "Pin Name" column as 'Gate name'.'Symbol pin name'.

     

    Do read the Manuals example of creating a device. The manual is found  in the Eagle folder "Documentation".

    The section "Component Design Explained through examples". (That's the correct section in v7.7)

     

    All the best

    Warren

Reply
  • 0

    Hello

    I believe you have not followed the library creation tutorials properly.

     

    It's  three step process.

    Create a package

    Create the symbols that will be used in the device

    Create a device using a previously created package and the previously created symbols.

    Only then will the "connect" dialog show pins of the device and pads of the Package (footprint)

     

    Have a look at one of the Eagle supplied libraries for a relay. (relay.lbr)

    Open relay.lbr

    Display the Device RT42?*

    You will see the Device is composed of three symbols and a package (footprint)

    Using the Information tool (I) you will see the names of the Symbols are "K" and "U".

    The symbol "U" has been used here twice.

    Each symbol placed into the Device is referred to as a "Gate"

    Using the Information tool (I) you will see the names of the gates are "1" "2" and "3"

     

    The pin numbers displayed in the device editor only appear after the "connect" is made. Prior to that they appear in the "connect" dialog "Pin Name" column as 'Gate name'.'Symbol pin name'.

     

    Do read the Manuals example of creating a device. The manual is found  in the Eagle folder "Documentation".

    The section "Component Design Explained through examples". (That's the correct section in v7.7)

     

    All the best

    Warren

Children
  • 0 in reply to WarrenBrayshaw

    Am 12.08.2018 um 01:53 schrieb Warren Brayshaw:

    Hello

    I believe you have not followed the library creation tutorials properly.

     

    It's  three step process.

    Create a package

    Create the symbols that will be used in the device

    Create a device using a previously created package and the previously created symbols.

    Only then will the "connect" dialog show pins of the device and pads of the Package (footprint)

     

    Have a look at one of the Eagle supplied libraries for a relay. (relay.lbr)

    Open relay.lbr

    Display the Device RT42?*

    You will see the Device is composed of three symbols and a package (footprint)

    Using the Information tool (I) you will see the names of the Symbols are "K" and "U".

    The symbol "U" has been used here twice.

    Each symbol placed into the Device is referred to as a "Gate"

    Using the Information tool (I) you will see the names of the gates are "1" "2" and "3"

     

    The pin numbers displayed in the device editor only appear after the "connect" is made. Prior to that they appear in the "connect" dialog "Pin Name" column as 'Gate name'.'Symbol pin name'.

     

    Do read the Manuals example of creating a device. The manual is found  in the Eagle folder "Documentation".

    The section "Component Design Explained through examples". (That's the correct section in v7.7)

     

    All the best

    Warren

     

    --

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

    https://www.element14.com/community/message/243267

     

     

    Well, everything has been said and I hope you have success now.

    What I'm doing here is to make it even more "complicated" image

     

    Generally for symbols one should use names (as you have done nicely).

    For the pads in the package one should use numbers.

    The pad numbers generated by eagle are like P$1, P$2... but have you

    ever seen something like that in a professional drawing?

    They are usually just 1, 2, 3... (but one can NAME them as one likes).

     

    For the pins something else is to consider, the DIRECTION.

    If the PIN layer is switched on (like in your symbol) one sees a (green)

      circle near the pin.

    In your case all pins have the direction "IO". Use the help function in

    eagle (help pin) and learn about the directions used in eagle symbols.

    For relay contacts I would use PAS(sive). IO are usually used for micro

    controller ports which can be set as input or output.

     

    The reason for this "unnecessary" work is the electrical rules check (ERC).

    This feature can not work correctly without correct pin directions.

     

    --

    Mit freundlichen Grüßen / With best regards

     

    Joern Paschedag