[SOLVED] how to highlight electrically connected tracks in altium

Status
Not open for further replies.

Fractional-N

Full Member level 1
Joined
Oct 15, 2007
Messages
97
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,288
Activity points
2,071
Hi,
I have a two sided complex and dense PCB document. the tracks has no net names. I want to highlight a net(track) to see where it goes inside the PCB, how should I do that? ["show net" does not work]
 

<CNTRL> + <Click on the net> works for me (Altium R13).

[ & ] change the contrast level.

HTH.
 
[ & ] change the contrast level.
Click to expand...
are you serious! kidding me?
---

select -> physical connection OR 's' and then 'p' then select the track. it would select all physical (electrical) connection the track is connected to. now is there a way to highlight the selected?
 

Nope, cntrl + click on the net or track highlights everything on the net (IIRC Enter cancels the highlight).
The brightness of the non selected things can be changed with [ (reduces brightness) and ] (increases brightness), the altium terminology is that it changes the mask level.

Note that this is not equivalent to a select operation this only highlights.

Is it just me or is the new select connected copper single layer command one off the most useful (and long overdue) commands ever.

Regards, Dan.
 
Thanks. I got it. but the problem is cntrl + click does not work in my PCB, because tracks in the PCB has no net name or they are not connected to any net. they are just simple tracks.
the best way for me to see where does a track goes is to use the select function of altium. as I already said select physical connection. then it will select all tracks connected to each other inside the PCB and I can see the electrical connection between tracks.
it would be very nice if I could highlight the already selected tracks but it seems that altium does not have such ability.
 

That is a horrible way to use a pcb cad package as it means that all the ERC and DRC functionality is unavailable to you (Seriously, draw a schematic first you will be much happier).

I think you can in fact dim the non selected tracks (Try '[' ) but it probably depends on what display mode you have set, memory is that <something> - S (Shift or control?) toggles around the display modes, it may also depend on your preferences settings.

73 Dan.
 
yeah it's horrible :-( , but i'm not the one who has drawn the PCB. I have an FPGA board and corresponding PCB & just want to figure out where the FPGA pins are connected.

No luck. shift+s hides (or shades) other layers.
 

Looks like gerber data or a similar artwork description has been imported to Altium. By nature of the "No net" copper features, they are excluded from DRC. I don't think that Altium (or another CAD tool) has a feature to extract netlist information from artwork. Some gerber tools however have it for test data generation.

If the PCB has been somehow regularly designed, there would be also netlist data that can be imported to Altium.
 
Create a schematic with a couple of hundred short unconnected nets, then you can work around the gate array doing esc (edit select connected copper) and then assign a net name to each selection (It might even be scriptable)?

Actually, create a schematic sheet with the appropriate fpga on it with each pin having a small net of sane name, that way you can assign meaningful names to nets.

The other approach to this sort of thing is to find the jtag pins and use boundary scan to figure out what is on the jtag loop and what you can trace out that way.

Regards, Dan.
 
Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…