Before trying to create or update a PCB, you should Validate your schematic. (Project > Validate PCB Project). This is also shown when you try to update the PCB. Errors can prevent the update process from working correctly.
The Messages panel (View > Panels > Messages) will list any errors and warnings that the schematic has based on the Error Reporting configuration under project options (Project > Project Options > Error Reporting tab).
The visible errors in your image are:
- Unknown pin
- Failed to add class member (under add component class)
Unknown pin
The unknown pins correspond to components which you've assigned the designators TERMOS and RELOJ1.
(Note that designators in schematics are commonly assigned using just one or two characters followed by a number. For integrated circuits or "chips" these are usually U. Instead of TERMOS, that component might be better designated U1. Connectors and jacks might be assigned CN or J, so instead of RELOJ1 it would just be J1.)
Do your symbols — the components in a schematic — have valid footprints associated with them? It appears that you have a symbol to which you've connected wires, but when you try to publish to the PCB, it can't find the appropriate pads that would be associated with its footprint. You should read up on how to create footprints.
When you say "I have checked the library and the pins and it is ok." what do you mean? Did your library compile without any errors? Have you verified the symbol pins all correspond to footprint pins? Refer to the link above (re: how to create footprints) if not.
Failed to add class member
The failure to add class members is a secondary effect of not having working footprints. When Altium adds a component footprint to a PCB, it (by default) also adds that PCB component to a component or room class based on the schematic sheet it is on. If the footprint were working, this error would likely disappear. Nevertheless, you may want to review how class generation works.
Other possible validation errors
Based on your images, I'll list some other potential issues:
Are you using a standard grid for your schematic editing? You have little kinks and bends in your wires which suggests you're having some problems here. Symbol pins and wires on the schematic can be difficult to connect properly if the symbol uses one grid pitch and the schematic editor uses another. It is highly recommended (but not required) to use 2.54 mm (100 mil) grid spacing for both. It's possible to have wires that look connected but actually aren't, which can result in errors during schematic validation.
Previous questions/answers related to this:
The Arduino in the center of your schematic still has a wildcard placeholder for its designator (*). As above, you should assign it a designator that you can use to refer to it, as well as avoid schematic annotation errors. You can maintain all the designators manually, or use the annotation tools.
Finally, there are lots of good resources on the web, but you may have missed them. In particular, you should know about and use:
There are also great users who've posted countless hours of content that often teach a great deal about PCB design and Altium in particular.
As you can see, there's a great deal of information that goes into answering your question. If you have further questions, you should use one of the resources above, or ask a new question. (Don't add a comment below to ask a new question.) Hopefully the information I've provided will help you narrow the problem down, and if you continue to have errors, you can post a new question that is specific to an error. Being specific is how to get definitive, useful answers.
