How can I edit the mask apertures settings?

There are two options available within DesignSpark PCB which globally control the solder mask and paste mask clearances around the copper pads of surface mount components as detailed below.

The clearances are set independently for each of the solder and paste masks.

The solder mask (resist) is set as a positive value to provide a clearance around a pad, this allows for some misalignment in manufacture and assembly to ensure the component lead will not have any obstruction for the solder connection to the copper pad.
It should not be set too large and resist should be present whenever possible between pads to avoid solder bridges.

The paste mask is used for the application of solder paste, i.e. it is not a physical part of the PCB, but used to produce a stencil with cutouts to allow the solder paste to be placed on the copper pad during PCB component assembly. Paste apertures are normally adjusted to be smaller than the copper pad area to ensure the paste does not spread outside of the copper area.

DesignSpark PCB has two options for setting the clearance values and these are within the "Design Technology" on the "Layer Types" tab. The options are "Absolute" and "Relative".

"Absolute" allows a fixed gap as entered in the "Size" column.

 This image shows an absolute gap of 0.1mm.

The value is entered in the design units and should be chosen to suite the size of the pads used within the design.
As an example for the solder paste, if a copper pad is 4mm x 3mm and a value of -0.5 is entered in the 'size' column, the aperture created will 3mm x 2mm, i.e. a gap of 0.5mm around the paste.

"Relative" (or percentage) allows the gap to be percentage of the pad size.

 This image shows a relative gap of 10 percent.

This option has the advantage when a design has a large variation in the pad sizes used, it allows a larger gap for large pads and a correspondingly smaller gap for small pads allowing more paste to be applied on the smallest pads than the Absolute option.  
Again using an example 4mm x 3mm pad size and a value of -10 in the size column this will create an aperture of 3.2mm x 2.4mm i.e. the gap is 0.4mm with 4mm pad length and 0.3mm with the 3mm pad width, hence the size of the gap is relative to the pad dimension.

Suggestions.

If you are an advanced user using the above options then it is an advantage to use a technology file and select the additional required layers when first using the PCB Wizard. Use the "Define Layers" option and add the paste and solder mask layers for ease of viewing and configuring.

 If you are mid design and you have not added these layers for viewing and configuring (they will still be produced by the 'Manufacturing Outputs") you can add these layers for viewing manually by following this FAQ How do I add a solder mask?