Altium Schematic and PCB Layout net connectivity check

[maxpayne]

I am wondering if there is any method available in Altium to check/verify if the components connection in schematic is same as physical layout connection in the PCB. In Eagle the PCB is updated instantaneously as soon as I update connections in schematic. But in Altium this is done by creating ECO.

Just  need to know the method of verifying that schematic nets and pcb nets are consistent and there is not any physical erroneous connectivity.

[ConKbot]

First, compile the project, make sure there isn't schematic issues, import changes from the project to the pcb, execute the ECO, make sure the drc rule for unrouted nets is enabled, then run DRC.

The compiling the project isn't strictly needed if you just tweak the schematic. And if you've been adding and removing components, check the component links to make sure all pcb components are linked to schematic components.

[free_electron]

Compilation not needed. Simp,y do D U.  design update pcb.
It will tell you exactly what, if any, discrepancies there arr and it will fix them for you.

[maxpayne]

Compilation not needed. Simp,y do D U.  design update pcb.
It will tell you exactly what, if any, discrepancies there arr and it will fix them for you.

Thanks free_ electron and ConKbot for your reply.

@free_electron,
Is there any other method apart from this ? The problem I faced is that sometimes I do make lot of changes (deleted, modified and replace) in the components/connections and there are lot of net differences showed up between the schematic and pcb when I do the (Project> show differences), then I have to manually match the nets which is a tiresome process.

[free_electron]

forget the net names. that resolves itself.

all you are after is checking removed parts, added parts and footprint changes. if that is according to what you want : run the ECO. (

workflow :

D-U
verify your footprint changes/removal/addition
Execute
Close

Go to PCB:

C - K       (Project -> Component Links )
push all to the right column by clicking "add pairs matched by" .make sure "designator is checked" , the rest is off".  if all is ok the left column should be empty. if not you have missing footprint or discrepancies between schematic / board : solve those in your schematic

D - N - A   Design-Netlist-Clean all nets
D - N - U  Design-Netlist-Update from pads
T - D -R  Tools-Design Rule Checker-Run

During layout only check the short circuit , unconnect and clearance rules. The rest is irellevant durign routing operations. You do want to run a full rule check prior to data out.

Once you get the report ( the HTML document) : close that. it is fancy but there is a much better way to drill into the problems.
Open the messages window. the same errors will be listed one by one. if you double click an error altium will directly zoom and highlight the offending elements on the PCB. you can click the + in front of the message line to get the details on what is wrong.

[T3sl4co1l]

Can also generate a differences report (this, and a DRC report, are handy additions to the OutJob -- see if there are any obvious oversights at the moment of output generation itself).

Tim

[maxpayne]

forget the net names. that resolves itself.

all you are after is checking removed parts, added parts and footprint changes. if that is according to what you want : run the ECO. (

workflow :

D-U
verify your footprint changes/removal/addition
Execute
Close

Go to PCB:

C - K       (Project -> Component Links )
push all to the right column by clicking "add pairs matched by" .make sure "designator is checked" , the rest is off".  if all is ok the left column should be empty. if not you have missing footprint or discrepancies between schematic / board : solve those in your schematic

D - N - A   Design-Netlist-Clean all nets
D - N - U  Design-Netlist-Update from pads
T - D -R  Tools-Design Rule Checker-Run

During layout only check the short circuit , unconnect and clearance rules. The rest is irellevant durign routing operations. You do want to run a full rule check prior to data out.

Once you get the report ( the HTML document) : close that. it is fancy but there is a much better way to drill into the problems.
Open the messages window. the same errors will be listed one by one. if you double click an error altium will directly zoom and highlight the offending elements on the PCB. you can click the + in front of the message line to get the details on what is wrong.

Thanks free_electron for your valuable suggestion. After DRC, I normally use PCB Rules and Violations to look for errors. This seems very handy to me.