Unkown pins when trying to pass from schematic to pcb

[senso]

Good afternoon, after deciding to try out Altium I have made a small schematic, and for some reason I'm getting this error:


I have already changed the pin designators in the footprint from the original(made by me, + and - to 1 and 2), the Pin Map shows the pins as maped 1 -> 1 and 2 ->2, i have already deleted and replaced those components but I still get the same error, and in the pcb, those 3 components aren't attached to any nets.
The relevant schematic is this part:

[senso]

Its getting even stranger I decided to delete the components and as expected it stopped giving those errors, but even adding a 1N4001 from the Standard Library gives the same Unknown pin and also this:


What is going on? 

[free_electron]

Changing in the pcb library does not do anything unless you recompile the integrated library.

There are a few steps involved in messing with the libraries.
what is thath 'res1' 'cap pol1' text that shows up ? are those part names ? you can't have space in part names or footprints ...

[senso]

For some components that aren't available in the Altium builtin libraries, like the ADc and the op-amps, and voltage references that I'm using I have created a PcbLib and SchLib files that have footprints and the schematic parts and all those work perfectly and I even learned how to add .step 3d models to them.

The res1 and cap pol1 are from the Miscellaneous Devices that comes with Altium, I haven't designed them.
You you say mess with the libraries, do you refer to alter the Altium ones, or when making a personnal library?

The strange thing is that the components that fail were made by Altium and not by me, but there is something fishy with the LM2576 or with some other thing, because I cant attach anything to the net that connects the pin 4 to the inductor.

[free_electron]

i never use the altium libraries. i copy parts from them in my own libraries. i don;t like the symbols used for the chips.
i typically re-arrange the pins so they make my schematics cleaner.

Now, the 'generic parts' library from altium is not an integrated library, so that is why yuo get the pin assignment errors.
copy the resistors and capcitors into your own library , link them , compile yor library and use those

[senso]

I have done that, and redone the footprints, and it finally works!

Thanks for the hints, the only thing I cant seem to find is how to compile a library.

[gxti]

Not sure that had anything to do with it, you just deleted whatever was giving it a tummyache. When import is behaving weirdly, the two things I do are 1) from the schematic, Project -> Compile PCB Project and 2) from the PCB editor, Project -> Component Links and verify that the left two columns are blank. If not, click "Perform Update" and it should sort itself out.

When you get that "match nets" dialog, just click the "Accept" button (or whatever it's called). It's asking if any of the new nets match against one of the nets that got removed, so you don't have to redraw the traces.

[free_electron]

To make an integrated library :
File - New Project- Integrated Library

Drag all your schlib and pcblibs in there ( you can have more than one i organize my parts in different schlibs and pcblibs. like Resistor 0603.schlib Resistor0805.schlib , Ic analog.schlib and so on. )

When done simply click Project - compile integrated library.
if you get warnings or errors : FIX ALL OF THEM.  NEVER EVER leave a warning or error in a library ! it will propagate to your design and come back and bite you sooner or later !

finally : add the compiled library to your library list.

[senso]

Thanks for the help Free_electron, you are a real life saver.

I have another doubt, is there a way to have automatic update of the poligon pours?
Its annoying to place a bunch of tracks and the double click in the poligor pour so it is regenerated, even Eagle can handle this, so it must be an hidden option or something..

[free_electron]

options - preferences - pcb - polygon repour threshold. set that to 50 or so.

the repour triggers when acirtain amount of 'imaginary traces' is crossed.
a polygon is made out of 'vritual traces with a certain width. what that width is i don;t know. as soon as you cross more than the threshold altium will repour the polygon. it will do that the moment you stopplacing the track so as not to interfere with your work.

[senso]

And yet again, thank you Free_electron.
I think I should pay you some beers 

I have another question if you dont mind helping me again, I have a pcb, that as some vias, and I would like to activate the tenting in the Vias, using the pcb list I can have a list of only the vias, but it doens't let me check the box to activate the force tenting I have to double click and edit the vias proprieties for each one, is there a faster way?

Thanks in advance.

[enz]

And yet again, thank you Free_electron.
I think I should pay you some beers 

I have another question if you dont mind helping me again, I have a pcb, that as some vias, and I would like to activate the tenting in the Vias, using the pcb list I can have a list of only the vias, but it doens't let me check the box to activate the force tenting I have to double click and edit the vias proprieties for each one, is there a faster way?

Thanks in advance.

Look at the top left of the PCB List, there is a text-label called View, click on it. Now you can change this to "Edit". This changes the pcb-list from view-mode ("read-only") to edit-mode.

Martin

[free_electron]

Simply make a design rule and set the via soldermask to a large negative number.

Or click on one via , right click - select similar , and in the inspector click 'override soldermask' and enter a large negative number for the override value.
switch to 3d view to verify they are covered .