Via NAME error

Alex Hunter wrote:

On my current design, I am having trouble naming vias using the NAME

command.  When I use the NAME command, and try to assign it to an

existing net (e.g. GND), I get an error: "Cannot backannotate this

operation. Please do this in the schematic!"

 

This does not make sense.  I should be able to rename the via. Any

suggestions?

if the via belongs to an already existing net (has the same name as),

you can't rename it in the board.

This would rename the net containing the via and so combine the two

nets.

This on the other hand  could change the schematic, which is only

allowed in the schematic editor.

Why do you need to rename via on the board at all?

If you want to place additional GND vias it is much easier to use "via

'netname" beforehand.

--

Lorenz

On 5/12/2013 7:25 p.m., Lorenz wrote:

Alex Hunter wrote:

On my current design, I am having trouble naming vias using the NAME

command.  When I use the NAME command, and try to assign it to an

existing net (e.g. GND), I get an error: "Cannot backannotate this

operation. Please do this in the schematic!"

 

This does not make sense.  I should be able to rename the via. Any

suggestions?

 

if the via belongs to an already existing net (has the same name as),

you can't rename it in the board.

This would rename the net containing the via and so combine the two

nets.

This on the other hand  could change the schematic, which is only

allowed in the schematic editor.

 

Actually, at least with v6.5, you can rename a via on the board and the

traces are renamed. Also the schematic nets are changed to match.

Which version is Alex using?

HTH

Warren

On 05/12/13 07:37, warrenbrayshaw wrote:

 

Actually, at least with v6.5, you can rename a via on the board and the

traces are renamed. Also the schematic nets are changed to match.

This is also true of V5, but only if you're renaming it to a new,

pristine, as-yet-unused name. If you try to rename a via that's on an

existing net to the same name as another existing net, then you've

joined two nets and this is a structural change to the schematic which

isn't allowed from the board editor.

warrenbrayshaw wrote:

On 5/12/2013 7:25 p.m., Lorenz wrote:

Alex Hunter wrote:

On my current design, I am having trouble naming vias using the NAME

command.  When I use the NAME command, and try to assign it to an

existing net (e.g. GND), I get an error: "Cannot backannotate this

operation. Please do this in the schematic!"

 

This does not make sense.  I should be able to rename the via. Any

suggestions?

 

if the via belongs to an already existing net (has the same name as),

you can't rename it in the board.

This would rename the net containing the via and so combine the two

nets.

This on the other hand  could change the schematic, which is only

allowed in the schematic editor.

 

 

Actually, at least with v6.5, you can rename a via on the board and the

traces are renamed. Also the schematic nets are changed to match.

even if two nets are combined that way?

... checking with 6.5.0 ...

nope!

renaming nets in the board editor only is allowed if the new name does

not exist yet, and there is not difference between renaming a trace,

airwire or via.

--

Lorenz

It sounds like that is the problem.  It is giving me the error because I am trying to combine two existing nets.

Why is the VIA command adding a via to an existing net? I don't think I've seen this behavior before.  I always could place a via (which would be assigned to a new net) and then rename it to GND.

I am using version 6.5.0.

Alex Hunter wrote:

Why is the VIA command adding a via to an existing net? I don't think

I've seen this behavior before.  I always could place a via (which would

be assigned to a new net) and then rename it to GND.

vias added without naming them beforehand (ie: via 'netname) even get

a S$... name and no N$... net name.

you are sure you used the via command in this case and didn't

copy/duplicate an existing one?

I am using version 6.5.0.

same here

--

Lorenz

The problem of not being able to name a via is new phenomenon (I'm using Eagle 6.4 - haven't updated yet).

I was always able to place a via (to stitch together ground planes) before, name it GND and be done with it.

This is a bit of rant but if Eagle would fix the things that are actually wrong with Eagle - such as a completely broken user interface,

before adding new and dubious features (I can't even call the Via bug a feature).  For beginners how about

Arrow keys that move things

An align and distribute dialog

Standard features now for just about every cad and drawing program.

How many person hours have been wasted because one can't change nets from the properties dialog?
Is there a reason for this except some kind of power trip to make people go to the name dialog.

Instead of a warning - why not just bring up the name dialog and be done with it.

addendum

After trying the VIA command   VIA 'GND'   for example, it does just want I want, but this kind of illustrates my point about

a broken GUI and UI. Why would I want to dig through a help file, that I don't have a clue which even exists, when

I can just add a via from a menu and give it a name. If you can do it from the command line, you should be able to

do it in an intuitive way from the GUI.  Maybe the programmers hate GUI programming. Even the import bitmap

menu item (which just runs the script  of the same name) is a welcome improvement that saves me having to scroll through

the same menus many times in the same day.

Paul Badger wrote on Sun, 23 March 2014 08:32

.....After trying the VIA command   VIA 'GND'   for example, it does

just want I want, but this kind of illustrates my point about a broken

GUI and UI. Why would I want to dig through a help file, that I don't

have a clue which even exists, when I can just add a via from a menu and

give it a name. If you can do it from the command line, you should be

able to do it in an intuitive way from the GUI.....

......Even the import bitmap menu item (which just runs the script  of

the same name) is a welcome improvement that saves me having to scroll

through the same menus many times in the same day.

I recommend you learn how to use the HELP. It is very good in v5 and v6

To address your last sentence  ".....If you can do it from the command

line, you should be able to do it in an intuitive way from the GUI."

1. I suspect you are not talking of intuition here but of a learned habit.

2. You can do it from the GUI

The PC cannot read your mind so you are going to have to tell Eagle the

name of the via at some point so why not name it before you place the via

rather than after?

If you provide a name for a via before you place it then subsequent vias

will have the same name. This saves renaming them individually. The most

common use of individually placed vias is for GND vias making this feature

very valuable.

So if you want 4 vias named GND

(1)Click the VIA icon (or from the drop down menu DRAW > VIA)

At this point the via is attached to the cursor but Eagle does not know

what to name it. You have to tell it.

(2)Type the name in the command line surrounded by single quotes. 'GND' and

hit

(3) Click 4 times to place the 4 vias , all named GND

And a comment on your final statement

Quote:

Even the import bitmap menu item (which just runs the script  of the

same name) is a welcome improvement that saves me having to scroll

through the same menus many times in the same day.

Eagle is very configurable. Efficient users will set up their environment

to suit their needs. So learn about context menus and Text Command menus.

For example, if CadSoft had not added Import Bitmap to the Menu system,

then you could have created a Text Menu button via the MENU command. All

those magical things the ULPs perform can be brought to a menu item for you

to click.  

All the best

Warren

--

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