Preventing Altium ECO from deleting things

[Mark]

I'm slightly embarrassed to even ask this as I'm sure there is a simple solution. 



There are often a number of items in the SCH (such as Z1, Z2, Z3, screws, nuts, washers and other HW items) that are added to the SCH because they will then show up in the BOM. 
There are some items in the PCB only with designators such as mounting holes (X1, X2, X3 etc). 
When going from SCH to PCB, the ECO wants to add the Z1, Z2 etc hardware to the PCB and remove the X1 X2 etc mounting holes. 

Is there a way to prevent this by changing a parameter for Z? X? components or by locking them? 

[ajb]

In the schematic symbol, you can define the component type:

Type - Select one of the following component types for the component footprint here. The available types are:

• Standard - components that possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. An example is a standard electrical component, such as a resistor.
• Mechanical - components that do not have electrical properties, are not synchronized (you must manually place them in both editors), and are included in the BOM. An example is a heatsink.
• Graphical - components that do not have electrical properties, are not synchronized (you must manually place them in both editors), and are not included in the BOM. An example is a company logo.
• Net Tie (In BOM) - components that are used to short two or more different nets together, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked; it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper within the component.
• Net Tie (No BOM) - components that are used to short two or more different nets together, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked; it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper in the component.
• Standard (No BOM) - components that possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. An example is a testpoint component that you want to exclude from the BOM.
• Jumper - components that are used to include wire links in a PCB design, for example, on a single-sided PCB that cannot be fully routed on one layer. For this component type, the component footprint and pins are synchronized between the schematic and PCB but the net assignments are not, and the component is included in the BOM. As well as selecting this option at the component level, both of the pads in the component must have their JumperID set to the same non-zero value. Jumper type components do not need to be wired on the schematic; they only need to be included on the schematic if they are required in the BOM. If they are not required in the BOM, they can be placed directly in the PCB where the Component Type is set, the JumperIDs are set, and the Nets manually assigned for the pads.

from https://www.altium.com/documentation/altium-designer/schematic-part-properties?version=19.0#!general-tab

That will solve a lot of problems like this.  You can also adjust comparator settings (Project > Project Options > Comparator tab) to cause Altium to ignore specific differences between the sch and pcb, but that's an extremely blunt instrument.  It would be an option if the design is finished as far as adding/removing components and you can't edit the types of the parts that are already in the design, though.