divide signal wires in schematics

[Marco Trapanese]

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

[KimP]

Post by Marco Trapanese
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

[SSFD SSFD]

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.

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/274734

[Warren Brayshaw]

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

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/275074

Attachments:
delete_net_wire.zip

[Lorenz]

Post by Warren Brayshaw
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.
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

[warrenbrayshaw]

Post by Lorenz
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

[Lorenz]

Post by warrenbrayshaw

Post by Lorenz
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

Post by warrenbrayshaw
It's the old problem. Element14 don't interchange attachments with the
news group so I'll attach it here.

thanks

[KimP]

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

[Lorenz]

Post by KimP
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.
- 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.

any idea how to use that from within a ULP without resorting to a
temporary script file?

I have found no way to get this sequence working from an ULPs exit
command

MOVE (>0 0)
EDIT .s2
(0 0)

Similar problem with layer selection during the attributes command

ATTRIBUTE
LAYER layer
partname attributename 'attributevalue';

[Chuck Huber]

Post by Marco Trapanese

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

[Warren Brayshaw]

Hi Kim

I'm using version 7.7 so your experience may be different to mine and for me there is one issue that makes the method unusable for me.

When I use your method (which is described in the HELP pages for the MOVE command) to delete a net wire, it all appears to go well but Eagle has not done it correctly. A bug I would call it.
Eagle keeps the net segment as a single segment, but the wire has gone. Because it's still one segment there is no need for a net name change for a portion of it.
This can be verified by looking at the XML of the schematic file.

Perform the following simple test to observe the problem with this:
Create a multi wire net segment between two pins.
Put a net label on the wires that attach to the pins. They will show the same net name at this point
Use your technique to remove a net wire in the middle of your the segment.
The net labels will remain the same
Now, normally, you should be able to delete the loose ends of the net/s (The ones previously attached to the wire you removed) with no detrimental effects. i.e. using the DELETE icon and the mouse to delete one of these wires.
What happens when that the wire is deleted, this divides the segment into two (finally) and the short segment is given a new new name.

The discussion has given me some ideas to check out so a better ULP may come out of it.

HTH
Warren

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/275216