How do I split a symbol/device into several pieces?

Am 26.12.2014 um 21:21 schrieb Max M:

I am working with a device that has 260 pins; if I begin to wire it, it

beings to get WAY too messy.

I was wondering if there was a way to break up the block into say 3

other blocks and wire that way. So instead of having say U1, I would

have U1a, U1b, U1c.

 

Also; I'm using the windows version of  the program and I only have a

week of experience with Eagle 7.2.0

 

Thank you very much!

 

--

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

http://www.element14.com/community/message/135881

 

HI,

this is matter of the library definition. A device can consist

of several symbols that you can place separately in the schematic.

Please take a look into the Library chapter in the manual. There

is an examople how to create a device that consists of several

symbol. Check the information about Addlevel as well. HTH

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

  FAQ: http://www.cadsoft.de/training/faq/

On 12/26/2014 03:21 PM, Max M wrote:

I am working with a device that has 260 pins; if I begin to wire it, it

beings to get WAY too messy.

I was wondering if there was a way to break up the block into say 3

other blocks and wire that way. So instead of having say U1, I would

have U1a, U1b, U1c.

You could break it up in that manner.  A technique that I have often

applied is to create a symbol for each into logical blocks.  For

instance, for a microcontroller, I might have a symbol that enumerates

the pins on P1, i.e. P1.0 ... P1.31.  Another symbol would host the pins

on P2.  I would also have a power block where all the power pins are

located, VDD@1, VDD@25, GND@2, GND@26, VDDIO, AGND, AVDD, etc.  If there

are special functions, like JTAG or USB pins, I'll put those in separate

symbols.

In the device editor, add each one of these symbols, and using the NAME

command, give each a different name.  In the above example, I might use

-P1, -P2, -PWR, -JTAG.  In this manner, when I add the device to a

schematic, the symbols would have names like U1-P1, U1-P2, U1-PWR, and

U1-JTAG.  If one were to name the symbols A, B, and C, they would appear

on the schematic as U1A, U1B, and U1C.  Lower cases letters are not an

option.

An example of this is in freescale.lbr.  Open it up and edit the device

MCF53*.

HTH,

    - Chuck

Wow that was incredibly helpful! Thank you very much.

I do have one more question; so i went ahead and created my chip as 3 symbols and 1 device. I made 1 symbol to be all grounds, 1 symbol all power sources and my final symbol is the rest of the pins. Is it possible to split up one device across multiple sheets? Because placing all three symbols onto one page takes up quite a bit of room as well. Thank you once more Chuck Huber!

On 12/29/2014 02:17 PM, Max M wrote:

Wow that was incredibly helpful! Thank you very much.

 

I do have one more question; so i went ahead and created my chip as 3

symbols and 1 device. I made 1 symbol to be all grounds, 1 symbol all

power sources and my final symbol is the rest of the pins. Is it

possible to split up one device across multiple sheets? Because placing

all three symbols onto one page takes up quite a bit of room as well.

Thank you once more Chuck Huber!

Yes.  This is described in the manual, but I'm not quite sure where.

First, you have to make sure your sheet thumbnails are visible.  To do

this, click right on a blank area of a toolbar and make sure "Sheets" is

checked.

Next, group the symbol that you want to move to another sheet.

Finally, drag the group with a control-right-click and click inside the

thumbnail of the destination sheet.  The MOVE command will continue

moving the group on the new sheet.

This does not work when dragging an individual symbol - it only works

when moving a group to another sheet.

HTH,

    - Chuck

A bit of clarification on Chuck's comment (I just went through this

"moving" experience).  You have to have what you want to move in a "group"

- even if that "group" is only one pin, it still needs to be first

"grouped" before you can move it to another sheet.  Chuck did say that, bit

it is easy to read over that part of the statement.  Look through the forum

here (I forgot to grab a link to it) - I had a post in the last few weeks

asking about moving symbols between schematic sheets.

mikey

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Once again; thank you very much chuck. That was very informative and helpful. I'm beginning to feel like a pro with Eagle Cad and your expertise.

autodeskguest Thank you as well. It's a little odd that you are not be able to move a single piece without grouping it, but oh well. Grouping it is!

On 12/31/2014 11:17 AM, Max M wrote:

Once again; thank you very much chuck. That was very informative and

helpful. I'm beginning to feel like a pro with Eagle Cad and your

expertise.

Glad to help.

Thank you as well. It's a little odd that you are not be able to move a

single piece without grouping it, but oh well. Grouping it is!

Well, it probably has something to do with a mouse drag.  When moving a

single component, you can drag it around while holding the left mouse

button down, which is a real live "drag" action from the perspective of

the underlying windowing software.  The object being dragged will follow

the mouse as long as the mouse remains within the work area.  As soon as

the mouse leaves the work area, say, over a toolbar or sheet thumbnail,

the drag suspends.  If one releases the mouse button while outside of

the work area, the component is dropped at the last valid coordinate

within the work area.

Contrast that with a group move where you do a Ctrl-Right-Click and move

the mouse around without any buttons held down, which is not technically

a "drag" action.  The Ctrl-Right-Click simply binds the group to the

mouse causing the group to follow mouse movements.  This allows one to

left-click inside the sheet thumbnail - something that can't be done

while dragging an object.

As a software engineer, I can see the significant difference between the

two actions.  Suppose the intent would be to drag a single component

onto a sheet thumbnail and drop the component there - a typical

drag-and-drop action.  I'm not sure exactly how the program could could

continue the "drag" after switching to the destination sheet since the

mouse button is no longer pressed and the component is no longer being

dragged.  The best way to accomplish this would be to start the move

command (type it into the command line, or click on the icon), then

click on the component to move, then click again at it's destination

location (perhaps on a sheet thumbnail) - a fashion similar to a group

move.  It'd be a programmatic change and a fundamental change to the

behavior of the UI, a change that I'm sure some would endorse while

others would condemn.  It would certainly generate a lively debate, to

be sure.  The upside to an approach such as this is that the group move

and non-group move would have the same architecture differing only by a

left-click versus a Ctrl-right-click.

It's something to ponder...

Best regards,

    - Chuck