Platform forum

Altiim 18, replace components in schematics

Juan , 02-26-2018, 01:11 PM
I want to change the components of the same value or same package in a sheet of a schematic or in all project, for example i have in a sheet of the schematic with 40 capacitors of 1uf and i want change all units to 4.7 uf, How i can do it?in Altium 17 i used the inspector, but in Altium 18 i don't find the way to do it.
robertferanec , 02-26-2018, 05:07 PM
This can help: http://www.fedevel.com/designhelp/fo...ect-components
In AD18, you may need to go to click on "Panels" button down in right corner (you need to be in schematic). You should be able to enable SCH Filter. Then you need to use Properties Panel to change the values (just change the value and press enter):

Juan , 02-27-2018, 01:02 PM
Thank you Robert,
godzich , 03-22-2018, 02:33 AM
Hi Robert,

First I want to express my respect for what you do in general, but especially regarding your Altium tutorials.

The selection of any components or their attributes is now really simple in Altium 18.

However, I am still looking for an elegant and fast way to replace singles or group of components in the schematic with other ones. Let's take as an example; a design that was started in a hurry by placing a bunch of 10k resistors from the Altium Content Vault all over the design as placeholders for all needed resistors. This is quite often a typical workflow - you don't have on hand all final values when you start the schematic entry. Now resistors here and there need to be changed not just to the final value by changing some attribute - but to the final Altium Content Vault component.

Having many years of experience with PADS. There it is fairly easy; you just select the component(s) in the schematic and right click and select "replace components". Then you pick the new component from the active library and you are done. Of course, you need to ECO the changes to the PCB but if the schematic and PCB decals are the same, there is no need for any additional routing or editing, the component(s) is/are just replaced with another one.

How do I do this is Altium 18? Is there an elegant and easy way? Such a pro application should have something similar, I have not found one...

Best regards,


robertferanec , 03-22-2018, 05:35 PM
Thank you @godzich. Normally you may want to use Update from Library (Tools -> Update from Libraries ...): http://www.fedevel.com/designhelp/fo...s-library-name

However, I am not sure if that will work for components from vault. Please let me know.
godzich , 03-23-2018, 08:11 AM

The mechanism you describe is to my understanding the one you use when you have updated some components in the library and want to reflect those changes to your schematic(s). Convenient but not suitable for the purpose of replacing schematic components (solely or in groups) with other ones. If there is no tool for that in Altium 18 it is a clear weakness. I will add a contribution and suggest this functionality to be added. I just thought that I could not find this function in AD18 since I'm still learning...
nieles , 08-08-2019, 05:42 AM
from AD 19.1 this feature is added https://www.altium.com/documentation...e-based)+))_AD

in AD 18 its also possible but a litte harder. first you need to look up the library name and new design item ID. then in excel you make a column with both texts and add a row for each item you want to replace. (see attachement) then you select the components in AD 18 and open the SCH list bar in 'edit mode' from the top left corner of the toolbar. next you 'smart grid paste' those items over the exsisting items in the 'library' and 'design item ID' columns.
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?