divide signal wires in schematics

Il 09/04/2013 12:11, KimP ha scritto:

I am aware that you can delete a middle segment of a wire and then

rename back the shorter part. The BIG problem is that if there also

exists a (consistent) routed *.brd file the wire delete in schematics

will also ripup some part of the routed wire in *.brd.

 

All this could be done by 1) closing the *.brd file, 2) ignoring "F/B

Annotation has been severed!" warning, 3) deleting wire, 4) renaming

back the shorter part, 5) reopening *.brd file, 6) running ERC to verify

consistency. Much easier/quicker/safer if there existed a

"Control+Delete" on wires (or similar command) in schematics editor...

A simpler workaraound is to add a third segment to the net and then

delete one of the other. In this way there is no need to play with the

(un)consistency.

Marco

Il 09/04/2013 12:36, Marco Trapanese ha scritto:

A simpler workaraound is to add a third segment to the net and then

delete one of the other. In this way there is no need to play with the

(un)consistency.

I don't think that works. I have tried several options, but found no

native way to separate schematic wires without getting net renaming.

True almost, there is one peculiar way it can be done:

Group the (subset of) wires and components you want to separate from

rest, move the selected group to another sheet. On the 2nd sheet you now

have the divided part of wires keeping their original name. Now, if

needed, this group can be moved back to the originating sheet. This

option would not work in Freeware editiom, having only 1 schematics

sheet available.

Kim

--

I am using the free version of SPAMfighter.

SPAMfighter has removed 193 of my spam emails to date.

Get the free SPAMfighter here: http://www.spamfighter.com/len

Do you have a slow PC? Try a Free scan

http://www.spamfighter.com/SLOW-PCfighter?cid=sigen

Hi Kim,

I completely agree.  I've been revisiting old schematics and cleaning them up is a PAIN.  I like your workaround of closing the .brd file and severing annotation, but there has to be a better way.

On 4/9/13 06:36, Marco Trapanese wrote:

Il 09/04/2013 12:11, KimP ha scritto:

 

I am aware that you can delete a middle segment of a wire and then

rename back the shorter part. The BIG problem is that if there also

exists a (consistent) routed *.brd file the wire delete in schematics

will also ripup some part of the routed wire in *.brd.

 

All this could be done by 1) closing the *.brd file, 2) ignoring "F/B

Annotation has been severed!" warning, 3) deleting wire, 4) renaming

back the shorter part, 5) reopening *.brd file, 6) running ERC to verify

consistency. Much easier/quicker/safer if there existed a

"Control+Delete" on wires (or similar command) in schematics editor...

 

A simpler workaraound is to add a third segment to the net and then

delete one of the other. In this way there is no need to play with the

(un)consistency.

 

Marco

 

I'm using Eagle 7.7.  The way I handle this is akin to Marco's suggestion.

I draw new net segments where I want the net to go, then delete the less

desired net segments.

HTH,

    - Chuck

On 4/9/13 06:36, Marco Trapanese wrote:

Il 09/04/2013 12:11, KimP ha scritto:

 

I am aware that you can delete a middle segment of a wire and then

rename back the shorter part. The BIG problem is that if there also

exists a (consistent) routed *.brd file the wire delete in schematics

will also ripup some part of the routed wire in *.brd.

 

All this could be done by 1) closing the *.brd file, 2) ignoring "F/B

Annotation has been severed!" warning, 3) deleting wire, 4) renaming

back the shorter part, 5) reopening *.brd file, 6) running ERC to verify

consistency. Much easier/quicker/safer if there existed a

"Control+Delete" on wires (or similar command) in schematics editor...

 

A simpler workaraound is to add a third segment to the net and then

delete one of the other. In this way there is no need to play with the

(un)consistency.

 

Marco

 

I'm using Eagle 7.7.  The way I handle this is akin to Marco's suggestion.

I draw new net segments where I want the net to go, then delete the less

desired net segments.

HTH,

    - Chuck

As discussed previously , deleting  a net wire from the middle of a net segment causes a number of events that need to be managed

In the schematic the most obvious occurrence is that one of the resulting segments will be re-named and needs to be manually re-named back to the original net name.

If the board  is also currently open to maintain forward/backward notation, routed traces will become un-routed.

So the manual process is:

Close the board (to prevent routed traces from being ripped up)

Delete the net segment wire in the schematic

Find which portion of the net segment that has had a name change

Rename that net segment.

Re-open the board

The attached ULP  automates the above

To prepare for the use of the ULP, simply RUN it. The ULP will create a context menu item named “Delete Net Wire” .

To delete a net wire, right click on it and select “Delete Net Wire”.

There are some things to be aware of

1. When the board reopens it is not restored to the size and position it was at but to the Eagle default size and position.
2. The board will only be closed and re-opened when a net re-name is required.
3. When deleting a net wire attached to a pin the board remains open so that this can be reflected in the board, as with normal editing.
4. When deleting a net wire attached to nothing, a free end,  the board does not need updating at all so is left open with no harm done
5. While the board is closed its undo/redo is inactive. At the same time the delete and re-name is happening in the schematic. Hence the two undo/redo list are not tracking each other.
   If you decide you deleted a net wire in error and wish to undo (ctrl-z [windows]) the delete action in the Schematic, the Schematic and Board immediately become ‘inconsistent’.
   This is a reasonable occurrence. Continue to Undo twice more and the previously deleted  net wire will reappear.
   Next perform an ERC check and you will see the green dot appear indicating the Schematic and Board are consistent.
6. The ULP can only be run in the Schematic and requires that the Schematic/Board pair are both open

I hope the attached ULP (zipped) is of value for those on older Eagle versions. It should work on version 6.0 and has been tested with Eagle version 7.7

Current Eagle versions are moving to use the 'Slice' command to perform net splitting but some recent reading reveals it was not splitting exactly on the grid so that needs correcting  before the feature is useful.

Let me now here if there are issues with the attached ULP.

Regards
Warren

Warren Brayshaw wrote:

As discussed previously , deleting  a net wire from the middle of a net segment causes a number of events that need to be managed

 

In the schematic the most obvious occurrence is that one of the resulting segments will be re-named and needs to be manually re-named back to the original net name.

If the board  is also currently open to maintain forward/backward notation, routed traces will become un-routed.

 

So the manual process is:

Close the board (to prevent routed traces from being ripped up)

Delete the net segment wire in the schematic

Find which portion of the net segment that has had a name change

Rename that net segment.

Re-open the board

 

The attached ULP  automates the above

looks like the attachment got lost

--

Lorenz

On 9/05/2019 5:09 PM, Lorenz wrote:

 

looks like the attachment got lost

 

Nope not lost, it's exactly where I left it, on the Element14 site.

It's the old problem. Element14 don't interchange attachments with the

news group so I'll attach it here.

Enjoy

Warren

---

This email has been checked for viruses by Avast antivirus software.

https://www.avast.com/antivirus

There is a way to separate schematics nets and keep the same (original)

name on both nets. You don't need to close the brd file, nothing gets

ripup'ed in brd and no inconsistensies are created.

You can achieve this by doing the following:

- in schematics page group-select a net segment in the position where

you want separate that net

- move this group to another schematic sheet (move command, mouse

crtl-right, drag to another sheet)

- you will see that the selected net segment is now moved to this other

sheet

- you also see that in the original sheet this net segment is now gone,

leaving 2 separate net segments with same name, still referring to the

same net, no ripup in brd, no inconsistency

- you can now delete the small segment that was copied away to the other

sheet.

Kim

warrenbrayshaw wrote:

On 9/05/2019 5:09 PM, Lorenz wrote:

 

 

looks like the attachment got lost

 

 

Nope not lost, it's exactly where I left it, on the Element14 site.

ah yes, didn't think of that

It's the old problem. Element14 don't interchange attachments with the

news group so I'll attach it here.

thanks

--

Lorenz