Altium, reserve (lock) designator

[zuzu]

It's possible to force some designators to be fixed, regarding all kind of annotate?

We have some resistor networks that can be swapped in PCB (due to better routing) so R4A can be swappe in schematic with R5C. Now, the PCB netlist will be updated but if ant annotate in schematic, the optimised netlist will be blown again.

The question is, after we establish that "this should be R5", can we lock somehow and still use annotate in schematic? I don't know how to explain better

Tnx,

 

[toohec]

Yes, you can lock designators (and the sub-part designators) of specific parts to prevent them from changing when you annotate the schematic.

First, it's best to assign the desired designators to the parts that you wish to have locked or pre-defined designator values. (If you already have already annotated the schematics once, you may wish to reset the entire schematic using the "Reset Schematic Designators" under the tools menu in the schematic window before assigning the specific designators; this will prevent the possibility of duplicate designators.)

Once you have specified the designators manually for your intended "locked" components, open the "annotate schematics" options under the Tools menu. In the annotate schematics dialog box, on the right hand side under the proposed change list area, you will see a column listing the current designator values (and the sub part designators if applicable). There are two check boxes next to each part, one in the "designator" column, and one in the "sub" column. Checking the check-box will lock the associated designator and prevent it from changing during annotation updates. (The sub-part check box will prevent the sub-part identifier (A, B, C, etc.) from changing.) Locked parts are greyed out in the list, so it makes it easy to identify. If you leave the part unchecked, then you are signifying that Altium may change the designator value. After you check the appropriate boxes, click "Update changes list" and verify the new designator values in the "Proposed" column are what you expect before clicking "Accept Changes". The parts that were checked should have the same value in both the current and proposed columns.

You may need to review the left side of the annotate schematics dialog box as well since that specifies which sheets to annotate, the order, and the starting designator value for the parts on each sheet. If you need any help on those selections or options, let me know. You can always refer to Altium's help about annotation here: https://techdocs.altium.com/display/ADOH/Understanding+Design+Annotation

Important.... if you already have parts placed on a PCB, make sure your component links between the PCB and the schematic are up-to-date before changing your designator values. Components Links is available in the Project menu in the PCB editor only. If your component links are not up-to-date before updating the designators, the PCB tool will be unable to track the changes automatically. If you haven't placed any components on the PCB yet, then you don't need to worry about this.