A solder mask (or solder resist) is a pads-only plot which may be oversized by a small amount, usually 5 thou or thereabouts. This plot can easily be created using one of two methods.
Technique 1 : Using Plotting To Generate The Output
Use the Plotting dialog (or one of the Output dialogs in version 5 or earlier) to generate a 'Pads Only' plot of the Top or Bottom electrical layer. By selecting a 'Pads Only' plot, the relevant 'Pads Only Plot' options are enabled on the dialog. From this you can select the Over or Under sizing (this option is also used for Solder Paste Mask plots) of the pads, and the pad types to be output. This type of plot can be auto-generated (and saved) as part of your plot job in version 6.
Technique 2 : Creating Specific Layers
The second method is to create a new layer called Solder Resist using the [Layers] option from the [Settings] menu, and to setup a new layer type using the [Layer Type] option. By setting up the layer type to have all pads except Vias available for plotting or display, these will be used for the solder resist. The Layer must then be created to have use this new Layer Type. Using this method enables the pad sizes to be controlled specifically on a one-by-one basis using Pad exceptions.
From the [Styles] option on the [Settings] menu, select the [Pads] tab. Select each of the pad styles in turn that are used by pads that need solder mask, select the [Add Exception] option and select the Layer to change (Solder Resist) and the new Width and Length to be used. You will need a plot for this layer, but it should be plotted as a normal layer (not "pads only"), because you do not need to oversize the pads in the plotting as they will already have been set to the desired size.
Producing Solder Paste Plots
The same techniques can be used to generate solder paste plots for your surface mount components. Use the options on the Plotting dialog to ensure that only the surface mount pads are plotted, as you will not want paste to be applied to through-hole pads or vias.