Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Eagle symbol Creation help needed

Status
Not open for further replies.

Mikebits

Well-Known Member
I managed to get into the symbol editor and create pins, see image.

eaglemake.gif
What I can't figure out is how to assign pin numbers, as this option does not seem to show up in the properties box or any other menu option. Anyone care to shed some light on this illusive pin number assignment problem I am having?

Thanks
 
Last edited:
You have to design a symbol, a package and then create a device. It is at the device stage you assign pin numbers.

Mike.
 
Awww, that sounds like a pain, so if I just want to create the symbol without the mechanical stuff I am out of luck? Darn, I wanted to just get the schematic stuff first and get back to the mechanical later. Oh well, thanks. :)
 
So it would seem that it may be better to call up another symbol with same mechanical parameters and modify it, is this difficult to do, or can I call a part from lib a and copy to my own user lib?
 
Find the package you need and select all of it with the outline box. Cut it and then create your new package and paste it in.

Mike.
 
Hi Mike,

please follow those steps:

1. Open (or create) library and put in symbol <new>, change 'Visible' --> 'both'

2. Create a symbol and name the pins as you desire, e.g. D0 through D7. (Pic1)

3. Create a package and name the pads accordingly, e.g. 1 through 8, mark pin no.1 as shown on Pic2. (Use 0 line width and create the arrow using 'polygon'.

4. Create a device: New --> device name and use 'add'. Select the symbol you've created and place it near the center coordinates of the screen. Type in a default name for the device, e.g. 'SV'. Assign package to the device. Connect pins and pads.
When finished the device should look like Pic3.

Regards

Boncuk
 

Attachments

  • CON-SYM.gif
    CON-SYM.gif
    8 KB · Views: 225
  • CON-PAC.gif
    CON-PAC.gif
    6.4 KB · Views: 226
  • CON-DEV.gif
    CON-DEV.gif
    8.6 KB · Views: 350
So I created my symbol okay. See image. I saved my image in my new lbr.
**broken link removed**

I found the package I need ssop28 in analog devices.lbr.
**broken link removed**

I tried using the group tool and copy, but when I try to paste in my lbr I get buffer empty message. There must be a way to point to a generic package from 1 lib to another.

Thanks
 
It's really stupid but you have to use cut for a group copy. Copy just doesn't work.

Mike.
 
Last edited:
Thanks, I got the package saved into my lib, now to see if I can get the Device portion done... This software really make me miss Mentor Graphics.
 
Thanks for the help guys, I created my first Eagle symbol, somewhat painful as it was. U3 is my new part. One more question, is there a way to get rid of the $ sign in between the U and 3 of the ref des? Thanks again. BTW the part is the AD9850 Analog Devices DDS part if anyone wants the lib file let me know. Itried to arrange the pins so it would make a neat layout on the schematic.

**broken link removed**
 
Last edited:
Hi Mike,

that's an easy one:

You forgot to "give" it a name. Click on the 'IC'-symbol when creating the device and give it a default name like 'IC' or 'U' as prefix.

Using the device it will be shown as IC1 or U1 if it's the first being used for the schematic, counting up to 'ICxx' or 'Uxx' (xx stands for the logical sequence of numbers as the ICs are being used.)

Boncuk
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top