Component Links - Part 1

Component Links in Altium are very handy when used properly. 

However there are ways to get in to trouble if you don't understand how Component Links work and how they become broken or even worst corrupted.

To stay out of trouble do NOT copy and rename a schematic sheet. Instead add a new sheet, copy and paste from an existing sheet to the new sheet then re-annotate the new sheet.  Cut and Paste can be used to reset the unique IDs,

First let's look at how the component links are created.

Suggested Reading:

Edit Component Links | Online Documentation for Altium Products

Suggested Exercise:

Place cap (C5) in a schematic, then look at the properties of C5.

Note the part (symbol) has a unique ID = FQMRRBKU and to the right is a Reset Button.

Obviously your C5's unique ID will be different.

click on image to view

Create a PcbDoc and push C5 to the PCB.

Next a look at the properties of C5 in the PCB

The part has a unique ID = \FQMRRBKU

FQMRRBKU = \FQMRRBKU is the component link for C5.

Again your ID will be something different, however they should be a matched set.

Now in the schematic let's change the Ref/Des from C5 to C6. 

Check the properties of C6 and note the unique ID = FQMRRBKU (same ID).

Now we can import the changes from the schematic to the PCB and using the unique ID Altium will automatically update (change) the Ref/Des from C5 to C6 where ID FQMRRBKU = /FQMRRBKU.

In a nutshell Component Links allow us to re-annotate (change) Reference Designators in the schematic, then push the changes to the originally placed parts the PCB.

Now let the fun begin:

Let's Copy and Paste C6 in the schematic





Let's keep the duplicate C6 and push the changes to the PCB.

Select the PCB > Design Import Changes . . .



Note that Altium is warning us that there are compiler errors.

Let's ignore the warning for now and execute the changes.

Now we have a duplicate a C6 in the PCB.



Let's delete the original (first) C6 which has ID = FQMRRBKU in the PCB.

Let's delete the duplicate (2nd instance) of C6 in the Schematic.

Now in the Schematic I have C6 with ID = FQMRRBKU 

Now in the PCB I have C6 with ID =  \TJABRXVV

So now we have C6 in both the schematic and PCB, however we destroyed the matching unique ID (Component Link).

Another way to break the matched unique IDs is to select Reset button in the symbol's properties.

Let's push the changes from the schematic to the PCB.

Right away Altium warns us that there was a failure to match 1 of 11 components.




We have three options

1 Automatic Matching
2 Manual Matching
3 Cancel

Let's work backwards starting with option 3.




If we select Cancel the Engineering Change Order dialog is displayed.

Note that we can select Validate Changes or Execute Changes.

To cancel without making changes select the Close button.

Next let's look at Option 2, Manual Component Links.

Now we are presented with dialog for Manual matching or un-matching any and all parts in the design.



It's up to you to correctly match the components (you are on your own).

At the bottom of the dialog there are options to Add Pairs Matched By >> 



The default option is by Designator, however there are options to include more constraints i.e. same Comment and Footprint.

If we select Add Pairs Matched By >> Designator, then select Perform Update the results will be the same as if we had selected Automatic Linking (Option 1).

Related Link:

Component Links - Part 2 

That's It !