Introduction

This description assumes that item with the non-standard mask is placed on the top side of the board, but is equally valid for the bottom side by using the relevant bottom layer instead whenever a top layer is mentioned.

Why would you need custom resist or paste layers? Simply put, the problem with the automatically generated solder and paste masks is that they are based on information in the electrical layers, and only allow for a global clearance, so a different technique must be used when more flexibility is needed. Secondly, where complex pad shapes are being constructed using a mixture of 'real' pads and copper shapes to extend the profile, prior to V20, the extra copper is ignored by the standard resist and paste plots. From V20 onwards, it's possible to set up the copper shape to be included, so extra layers may not be necessary (See FAQ for non-standard pads). A third possibility is where tracks or copper need to be kept clear of resist, perhaps for testing, but more commonly where a structure must be soldered down, such as a r.f. screening can. Text added to a resist layer will appear as a void allowing underlying material (usually arranged to be copper) to show through. When non-standard resist clearances, or paste masks are required, the approach is to create the extra layers as required, then use pad exceptions on the relevant layer(s) to redefine the resist or paste. For this to work, it's really important that any relevant pads are defined as [Top], [Bottom] or [All] layer, because if they're only defined for an electrical layer, they just won't be present on any new layers! Because Easy-PC only allows one top and one bottom electrical layer, the new layers must be a non-electrical type. An inner layer would not do, as surface mount pads will only exist on the top (or bottom). Standard resist and paste mask plots cannot be generated from non-electrical layers, so standard plots must be used when outputting these layers, so the pad sizes will need to reflect the actual hole diameter required in the mask. The description assumes that a solder resist mask is being created, but differences where it's a custom paste mask are noted.

Technique

Versions prior to 9:

Go to [Settings], [Layers], and select [Layer Types]. In the layer type dialogue, select [Add]. The new layer type needs an appropriate name (such as 'Resist' or 'Paste'), and should include all pad types for which a solder mask hole is required. Thus 'Surface Sym. Pads' and 'All Layer Sym. Pads' are essential. 'Pads' is desirable, for mounting holes, and 'Vias' is optional. A 'Paste' layer type will only require 'Surface Sym. Pads'. Usage, of course, will be 'Non-Electrical'. Click on [OK].

This returns you to the 'Layers' dialogue. Select [Add]. The new layer will need a name such as 'Top Resist' ('Top Paste'), type will be 'Resist' ('Paste') or your equivalent, side will be 'Top', bias 'No Tracks', usage 'Non-Electrical', and no net name. Choose a suitable colour, and click [OK]. The new layer will appear. Use [Up] or [Down] to move it if you wish to a new position. Click [OK] again to close the 'Layers' window. Now go to [Settings], [Styles], and select the {Pads} tab. For each pad style, add a pad exception for the new layer. For each pad exception, (but NOT the main pad definition) increase the pad diameter by twice the desired resist clearance ('Paste' reduce by the desired paste undersize), except for the pad style used for the custom pads. This must be changed to the correct diameter for the solder resist/paste mask opening, as defined in the data sheet. Click on [OK] to save the changes.

Versions 9 to 11:

Go to [Settings], [Layers], and select [Layer Types]. In the layer type dialogue, select [Add]. The new layer type needs an appropriate name (such as 'Resist' or 'Paste ), and should include all pad types for which a solder mask hole is required. Thus 'Surface Sym. Pads' and 'All Layer Sym. Pads' are essential. 'Pads' is desirable, for mounting holes, and 'Vias' is optional. A 'Paste' layer type will only require 'Surface Sym. Pads'. Usage, of course, will be 'Non-Electrical'. Tick the 'Oversize' box, and make the pads larger by an absolute amount equal to the pad to track spacing for the design. (For 'Paste' use the percentage of pad width option, which will typically be undersize by about 20%). Click on [OK].

This returns you to the 'Layers' dialogue. Select [Add]. The new layer will need a name such as 'Top Resist' ('Top Paste'), the type will be 'Resist' ('Paste') or your equivalent and the side will be 'Top', bias 'No Tracks', usage 'Non-Electrical', with no net name. Choose a suitable colour, and click [OK]. The new layer will appear. Use [Up] or [Down] to move it if you wish to a new position. Click [OK] again to close the 'Layers' window.

Now go to [Settings], [Styles], and select the {Pads} tab. For the custom pad style only, create an exception on each resist (or paste) layer. The pad size must be changed to the correct diameter for the solder resist (or paste mask) opening, as defined in the data sheet. This will be treated as an absolute figure. No allowance is necessary for the oversize applied globally to these layers. Click on [OK] to save the changes.

Version 12 and later:

Follow the instructions for Version 9 to 11, but the relevant menus are [Settings], [Design Technology], then the 'Layer Types' and 'Layers' tabs. There is no longer any need for a link from the layers screen to the layer types screen, so just go directly to the relevant tab. When you have finished with a tab, select any others as needed. You can click on [Apply] to save the changes, but do not click on [OK] until you have finished.

Now continue:

Go to [View], [Display], and turn off all layers except the new one, to check that the pad sizes are correct for the solder resist or paste mask. When you create the Gerber files, the holes MUST be filled on the plot of these layers. These Gerber files replace the relevant resist or paste masks in the job, so delete any plot definition for the original resist or paste masks. Because the over or undersize parameters have already been applied to the pads, DO NOT use the 'Pads Only' option on ther 'Settings' tab. You may also find it useful to add a comment to the '.rpt' report file to explain how the new Gerber is to be used.