solder mask missing on some components

So if you use the command Tools - Padstack - Modify Design Padstack then click on one of the pads that is missing mask then right click - Edit, Padstack Editor will launch and you can add a definition for soldermask. Even if you copy the design pad size so it's one for one. Once complete use File - Update to Design and Exit and this then updates the padstack in the board file with a mask definition. Continue working through the pads that need this. The ideal scenario is that you edit the actual library padstack so that next time you use this padstack it has been updated to suit.   

Thank you for helping.  New to pcb editor and  I am so confused. 

Some of the items in yellow are components with pads that should not be masked. others are vias that I would think need to be masked.

Could you briefly explain the problem they are reporting? Components are missing soldermask openings vs solder mask?

So soldermask is an opening, you define an opening in padstack editor for items that you don't want soldermask on. When you send this to the fabricator he makes a negative of this to create a soldermask film, they then print soldernask on the board leaving your pins clear of soldermask (if that makes sense). Vias - depends, sometimes users want these covered with mask sometimes not, sometimes only one side. You may also need to generate a pastemask (where solder is printed on the pads) for automatic assembly. Hope that helps

Thank you for your patience and detailed responses. I believe I am making progress now.

I was able to make the changes using "Modify Design Padstack".

So, changes will remain until I use those parts in a new layout?

Otherwise I should use "Modify Library Padstack" for reuse in other designs? Is that correct?

Almost but the Modify Library Padstack only opens the library defined pad (so if you have a 6 layer design a PTH pin will only show the DEFAULT_INTERNAL layer rather than all 4 internal layer names. When you edit the pads if you want to make a permanent change just use File - Save in Padstack Editor before you update to the design and this will write the library padstack. 

They recommending that I unfill the vias.

They are suggesting I change it to this:(ideally, not a must)

How do I remove the filled vias? should I since they are isolated from the plane anyways?

Why are arrows pointing to the connectors? Does that mean they are connected to the plane unintentionally?

They recommending that I unfill the vias.

They are suggesting I change it to this:(ideally, not a must)

How do I remove the filled vias? should I since they are isolated from the plane anyways?

Why are arrows pointing to the connectors? Does that mean they are connected to the plane unintentionally?

Its unlikely to be the plane is connected incorrectly to the via since you would see a DRC error, Are the Shapes Up to Date (Check - Design Status). Sometimes connecting a pin to a large plane directly can be an issue since it can cause solder issues but unusual for a comment on a via. I would ask for an explanation from the fabricator