Is there any way of altering the pin numbers of library relays?

Question

I am using a relay from the library list under relays.

It is LY40 and the diagram looks identical to the relays on the circuit I am trying to produce a schematic for. Unfortunately the pins are all wrong, my coil is on pins 13 and 14 instead of pins 1 and 2.

Is there any way of changing them? Has anyone any info about making my own library items, maybe I could load the relay and alter it that way?

Thanks,

bob

kikoun · Accepted Answer

hi, 
 why is it that a number that appears in the schematic is only changeable on the package page 
 The "pad" name is changed in the package page because the pad name is related to the package only: For an example, you have a library with 2 logic devices, first one is a quad 2 inputs OR gates (74HCT32) and second one is a dual D flip-flop (74HC74). Each device have is own symbol, but both have the same package (SOIC-14). So in your library you have 2 devices, 2 symbols and only 1 package that used by the 2 devices . In the first device, the pad named '1' of the package is connected to the pin A in the symbol of the first gate (one of the 2 inputs) In the first device, the pad named '1' of the package is connected to the pin named !R in the symbol of the first flip-flop (reset input). As you can see the ' pad name ' is related to the package, and have nothing to do with the symbols. When you create a package you have to forget the symbol, because a package can be use by very different devices. And for the symbol the same applies too : often a same component exist in several packages. and a pin !R of your symbol may be connected to the pad '1' in the "DIL" package version, but connected to pad '16' in the QFN package version. Even if the pad name is not link to the symbol, it's common to show it on the schematic, because it's easier when you need to debug your board Is there any way of moving the pad name about in the same way? I don't think so, That's a limitation of Eagle....

kikoun · Answer

Hi, First point: When you edit a symbol in you library, on each pin you can select some parameters (open the properties window on the selected pin). The ' Visible ' parameter let you select if you wish to see on your symbol : - the ' pin name ' (name of the pin in the symbol ), - the ' pad name ' ( name of the corresponding pad of the package ). - both - no names at all. If you alter the pin name, and if the pin's Visible parameter is set to ' PAD', you will never see any change ! Same way, if you alter the PAD name, and if the pin's Visible parameter is set to ' PIN', you will never see any change ! Second point. In a Project, when you place a part from a library, Eagle copies the part from the library into the board and schematic. So if you edit later this part in the library, the changes will NOT be visible in your project, since the project will still have the previous version. So, if you want to apply the changes, you have done in a library into a project, you have to : - Open the project (board and schematic), - In the control panel, browse and found your library, and proceed a right click on the name of your library, then select "Update'. I hope it helps... Guillaume.

matelot · Answer

Thank you for the reply Guillaume. I am aware that the project stores the library item . I have opened a new project and on the empty schematic page, added my relay and tried all sorts of ways to alter the "pad" name as I now know it has thanks to your thread. I have now been able to alter the numbers, why is it that a number that appears in the schematic is only changeable on the package page? The schematic I am trying to produce is very well populated and being able to smash each component and move the names and values around each component is very useful. Is there any way of moving the pad name about in the same way?