hello, please help with these beginer questions ( drawings )

As earlier responses said, you really need to read through the tutorials.  I also hate to add that if you haven't done mechanical drawings before, you really need to read up on how they are to be done.  People have been doing drawings for a long time before CAD.  CAD makes it much quicker and neater, but doesn't really do it for you (auto dimension tries, but will only do it correctly if you design the Part "correctly").

It's always amazing how new Solidworks users always seem to want to do things that people who have used it for years just don't do, or that it seems that Solidworks won't handle.  That should tell you something.  Almost anything CAN be done in Solidworks, but it is set up to do most things correctly with a minimum of work.  Hence, anything that requires a lot of playing around with is likely not what most people want to do!

With regards to your specific questions I will attempt to comment on them:

1) if there are 3 equal circles, is it possible to make the 'x3' appear automatically ? or i have to dimension one of them, then edit it, in order to add the 'x3' ?

Yes, if you created the holes using the "Hole Wizard" and then use the "Hole Callout" tool to dimension them.  Otherwise, No.

2) is it possible to change a view scale quickly ? like select view + mouse scroll/drag corners ?

What's too slow about right clicking on Sheet1 and setting the Scale?  In general, your drawings should stick to a single scale as much as possible, except for Details.  And those usually default to twice the Sheet Scale but can also be changed at will.

3) is it possible, once i have used an user defined scale, like 1:0.5, to make it stay like that, instead of auto-changing to a predefined custom scale (2:1 in this case) ? if i wish to change it smoothly, to 1:0.55eq, i have to delete the '2:1' and type '1:0.55', instead of simply adding a '5' to '1:0.5'

Again, sounds like you are trying to change scales View by View.  Most users will set it for the Sheet and leave everything else to use the Sheet Scale.  Yes, you can't change the pre-defined scales.  You have to change to User-Defined, then you can do what you want.

4) is it possible to create a text/anotation with tolerance ?

Isn't that what a Dimension is for?  If you REALLY need to do this (unlikely) you CAN start a Note and then insert a dimension into it by clicking on an existing dimension.  You will get the complete dimension, including prefixes and postfixes, and it will update with the dimension.  You can even then hide the original dimension if you want.  But, I will say, that in hundreds and hundreds of drawings I can't really remember the last time I needed to do this.  Usually, you put in a dimension, and add needed information in the pre or post-fix text blocks.

5) is it possible to create a dimension with a single tolerance, without showing '0' for the missing one ?

Again, why would you want to do that?  It doesn't match any drawing Standard I'm aware of.

6) in order to display mass and material, inside the *.SLDDRW, is required to create those properties inside the *.SLDPRT file; do i have to re-create those propertries for each new *.SLDPRT file, or is there a way to make them default ?

Default properties can be set in your templates.  If you don't have anyone else using Solidworks who understands these you will need to read up on this.  At minimum you should have templates for Parts and Assemblies (probably in both Inch and Metric units if you use both) and Drawing Templates for the sizes you most often use, also in both Inch, and Metric and in whatever Standard you want to use.  Getting these set early on will make your life much much easier later.  If it is just you then whoever you bought Solidworks from may be able to set you up with a set.  If not, do some Googling and you will probably find some to start with.  The defaults that come with Solidworks are not very useful as is.

7) sometimes, inside a breaked view, some dimensions, like ordinate, etc, go crazy  i don't know why, but it happens, and if i have details from those views, those will go crazy as well ...

We'd have to see it.  Are you using the Drawing Break View commands?

8) if i have a view with 2 details, is it possible to make them all stick togheter ? like, if i move the detail, to move also the other detail, and the parent view ? similary, if i move the parent view, also, the details, to move automaticallly ? something like creating a 'group' of views ...

Projected Views are aligned to move together in the respective axes. Holding <Shift> down will move them together.  Details are not set up to do that but you can always <Ctrl> Select several views and move them together. 

9) how to exclude from automatic update ? let's supose, that only for one view, i wish to supress some features, while the others to reflect the full build; so far, i couldn't figure it out ...

Not quite sure what you want to do?  Are you trying to get one view without a feature and then a second view after you add it?  If so, you do that with Configurations in the part file.  One configuration has the feature, one has it suppressed.  Then you just choose which configuration which view shows.  Typically, people WANT views to stay current with the model!  Being able to turn it off would lead to dangerous mistakes.

10) 3 more questions inside attached photos

Not sure what you are trying to achieve in #3.  Are you trying to get cross hatching?  Why?  Blown up Details don't typically get hatched.  Also, It looks like you are breaking your part in both axes.  Unless your part is really strangely shaped I can't imagine breaking a cylindrical part in both axes.  It gets too hard to imagine what the real part looks like.

In #2 the answer is that you can change the arrow heads (under Leaders in the Dimension properties) to many other types, except the one you show.  The closest is a filled in arrow.

In #1 the answer is that it is more or less doable, though I can't imagine why you would do this as it does not meet any Standard at all.  You create the standard dimension, with arrows out and the Dimension where you want it.  Then right click on the lower Dim line and choose to "Hide Dimension Line".  Then right click on the lower extension line and choose "Hide Extension Line".  I'm sure you could even set this as the default in a template.  But I can't imagine doing this as Standard.