Replacing all instances of a part in a design?

[grahamUTKMN]

Is there a way to replace all the instances of a particular part within a design without having to do each part one by one?

Thanks,

Graham

[jorge_garcia]

Hi @grahamUTKMN,

I hope you're doing well. Yes you can.

First you need to form a group that consists of only those components you want to replace. Then in the inspector you'll find the replace quick action at the bottom, click it, select the part you want to replace it with and click OK. Bam!

How you form the group warrants some explanation. You'll want to set the selection filter to only select devices. You can also use the Design Manager and it's filter options to form very granular groups. The selections don't cross sheets so you'll have to do every sheet individually.

Let me know if there's anything else I can do for you.

Best Regards,

[grahamUTKMN]

Hi Jorge,

Thanks for the reply, that's made it a bit quicker.

I'm still strugging to the the device symbol to update though. The new symbol has more visible attributes than the one I'm replacing. I've had this in the past. I used to update the part, then click the 'Reposition Attributes' button and the new attributes would appear. This doesn't work any more - and I think might have been linked to me updating the version I was using. I was on an older version until I finished a design, then I updated to the latest.

Is this a known bug? Is there a work around?

Running 9.5.2 premium on a Mac.

Thanks,

Graham

[grahamUTKMN]

Does anyone know what I can do here?

Thanks,

G

[grahamUTKMN]

So does this feature simply not work?

Graham

[jorge_garcia]

Hello @grahamUTKMN,

I hope you're doing well. This feature should work, since nothing has changed in that code as far as I know.

What happens if you try to bring in a new instance of the part? Does it bring in those visible attributes? In one of the parts that isn't showing the attributes, click on it with the attribute command. Do all of your expected attributes show up?

Let me know if there's anything else I can do for you.

Best Regards,

[jjm17XBGQ]

You can change it in the library and update this lib

[grahamUTKMN]

Hi @jorge_garcia 

Thanks for your reply.

If I bring in an instance of a new part it brings it in correctly with the new attributes visible.

Do you mean the re-position attribute command? That used to work as that's what I did on a previous design. When I replace a part in the design now and then click on it with the reposition attribute command, the new attributes don't appear.

Hi @jjm17XBGQ 

If I update the library it also does not show the new attributes.

I've attached a picture of two caps that are the same, but I can not get the attributes to update on the old one.

Thanks,

Graham

[jorge_garcia]

Hello @grahamUTKMN,

I hope you're doing well. That's really weird, if you do a group Repostion command (make sure the command is set to restore attributes) does that work?

I'm not surprised that the update didn't work, depending on the differences between parts it may not be able to do an update. However, replace should almost always work .However, if even that should fail then manually replacing parts would be the way forward.

Let me know if you continue to run into problems

Best Regards,

[grahamUTKMN]

Hi @jorge_garcia 

Sorry, what do you mean by a group Repostion command?

I haven't actually edited either the schematic symbol or the footprint for these parts, just added visible attribute text in the schematic symbol so that designs are easier to review.

I tend to work on designs that bring in blocks of already designed circuitry, or even start off with an existing design and modify it. If I manually replace a part in a schematic it removes it from the PCB! I really do not want that! Is there a way around that?

Thanks,

Graham

[jjm17XBGQ]

" If I update the library it also does not show the new attributes."

Oh, that's bad. Than you have to use replace instead.  That runs into the same problem, touching every single element.

[grahamUTKMN]

Hi @jorge_garcia ,

I have an update for you.

If I select the 'Reposition Attributes' command on the right hand tool bar, and click a part I have replaced all that happens for me is the reference designator moves position.

If I select a part, right click and 'Restore Position' (which has the same symbol) then it works and I see my new attributes 🙂

Running 9.6.0 Premium on a Mac.

Does that help?

Graham

[mtl_asm]

Is it possible to share the library part or a screen shot of the device and symbol from the library?

I tried doing this,adding an attribute to the device and part, and clicking "reposition attributes" then left clicking on the part makes the new attribute appear. (i have 9.4.2)

Right clicking and selecting the option you mentioned _also_ makes the new variable appear.

The option you found might still be able to be run on a group because it should be the equivalent of a "shift + click" on the part (see help reposition). So to try it on group, just type this in command line

group all; 

then press enter

reposition (s> 0 0);

then press enter

See if that works. I cant tell because on mine both Reposition and  Restore position have the same effect in that the new attribute is added. 

So the steps i follower were:

Add attribute to device in library

Add attribute text field to symbol in library.

save library

update all library  in schematic 

use reposition attribute or restore position on said parts and the attribute apppears.

also just fyi regarding this:

"If I manually replace a part in a schematic it removes it from the PCB! I really do not want that! Is there a way around that?"

This is not true actually.  If you use the "replace" command, then the new part is positioned on the pcb the same place/orientation/connections as the original. Try it on a copy of one of your projects to see.

[grahamUTKMN]

Thanks for your reply trying to help.

*The option you found might still be able to be run on a group because it should be the equivalent of a "shift + click" on *the part (see help reposition). So to try it on group, just type this in command line

*

*group all;

*then press enter

*reposition (s> 0 0);

*then press enter

I tried what you suggested and it just has the same affect as the button on the left toolbar.

*So the steps i follower were:

*Add attribute to device in library

*Add attribute text field to symbol in library.

*save library

*update all library in schematic

*use reposition attribute or restore position on said parts and the attribute apppears.

Yes, I do the same, but only the option on the right mouse button actually works.

If I do 'CMD + click' to select more than one part, then use the right click option, the new attributes only appear for the last part selected.

I'm having to do them one by one and it is very time consuming!

Thanks,

Graham

[mtl_asm]

Does it work if you use "replace" 1 by 1? It seems like this was never clarified.

You said if you add a new part it has the information, what happens if you  use replace and replace it with the same part?

[mtl_asm · Accepted solution]

hi,

i found some new info about the "Reposition Attributes" button. If you click on it you will see in the menu bar now there is a menu with 4 options.

Restore Default

Name 

Value

Name & Value

If you have the "Restore Default" option, it acts as the "Restore Position" option when right clicking on a part. 

As you said earlier, clicking the "Reposition Attributes" button with the other options selected will reposition the name/value designator (according to the button to the right of the menu).

Also it works with group. So you can select all the parts you need to change, then select "Reposition Attributes" and change the option to "Restore Default" then right click and select "Reposition: Group"

Then it will change all at once. 

I checked with 9.6 it seems to work, just the reason both buttons worked the same for me in my previous post, and why for you it makes the name/value move  is likely explained by the selection in this "Reposition" box/dropdown menu. When i pick some other option it behaves as you described. 

If you look at the .brd in xml, basically when you call "update all" from  the libary menu after modifying the part as we described previously, it will add the "attribute" sub element to the <part> elements, but it does not add them to the <instance> elements (which seems to be necessary for them to render on the screen). Once you use "Restore position" on the part it does add the "attribute" sub element to the instances. Maybe they can update that in the future, or maybe there is a reason they don't. If you add a new part as you said earlier, the extra attributes do show up, and when using "add" the attribute sub element is added both places in the xml right away.

[grahamUTKMN]

You sir, are a hero!

That's sorted it!

That has saved me soooooo much time and stopped me going slightly mad while I'm working from home all on my own.

Thanks,

Graham

[scottH36AU]

I know this is an old thread, but this functionality no longer works in eagle as far as I can tell (V 9.4.2). You can now only replace 1 part at a time. Seleting a group of the same part, then Replace and picking the part to replace with results in only 1 part being changed. I just editing the files in the end to replace the parts. Doubt it'll ever be fixed.

[mtl_asm]

im not sure that replace ever worked on a group, but i might be misremembering.

if you wanted to achieve that though you could quite easily just making a ulp that generates a script with a replace command for every part in the current group. this would be relatively simple.