www.eda.co.uk

In Altium Designer Service Pack 3 we have a number of different methods we can use for Cross Probing between editors, using either the Schematic or the PCB objects to locate and/or select their PCB or Schematic counterparts.

Ideally these cross probing features would be used with a dual screen setup as you can have your schematic editor on one monitor and your PCB on the second.  However, these feature can still be used and useful with a single screen.

If you wish on a single screen setup you can tile or split your PCB and schematic editors so that you can view then both at the same time.

Splitting the main design window can be achieved by Right Mouse Clicking on the Document Tabs at the top of the, more information on this can be found under Help >» Getting Started » Welcome to the Altium Designer Environment, page 7.

Cross Probing

Cross probing in its simplest for can be achieved using the command Tools » Cross Probe or using the button from either the schematic or PCB editors.

Which the Cross Probe tools selecte you will have a cross on your cursor.  Using split or dual screen you can now click on a component in your Schematic and the equivalent component will be highlighted in PCB with the rest of the objects masked out.

If you are not using split screen or a dual monitor setup you can still use the cross probe to good effect, with the Cross Probe tool active, while clicking on the components in your schematic editor hold down the Ctrl key.  Holding the Ctrl key will change the focus from the schematic document to the PCB document.

You will find that you can use the Cross Probe tool from either the Schematic or the PCB editor plus you can select any object to cross probe not just components, be it a net/wire or Pin/Pad.

Cross Select Mode

Using the Cross Select Mode allows you to select one or more components in the Schematic and the equivalent PCB component will also be selected. To turn this option on use the command Tools » Cross Select Mode. With the option turned on you can select your components in the schematic using the normal methods to select the same component in PCB.

This option is also available from the PCB editor using the same command Tools » Cross Select Mode.

Selecting PCB Component

A second method of selecting the components in the PCB using the schematic is a command call Tools » Select PCB Components. This is very similar to the Cross Select Mode, select your components in the schematic editor and then perform the Select PCB Components command to select the components on your PCB. This tool is only available from Schematic to PCB.

Navigator Panel Cross Probing

Our final method, and probably the most powerful is to use the navigator panel to perform the cross probing. Again this is best used if you have a dual monitor setup or split screen but it will still work well on a single screen also.

Open a Project and use the Project » Compile PCB Project... command so that you Navigator panel is populated. Then from the within the Navigator panel you can select a component, net, pin etc...and if you hold down the Alt key whilst selecting your object the same object or set of objects will be selected in the your PCB document.