Frequently Asked Questions
Glue mask for flow soldered SMT
[ PCB Design / Design for Manufacture ]
When flow soldering surface mount components, they MUST be glued in place, as the pressure of the solder wave will otherwise just remove them from the board. The amount of glue will vary depending on the size of the component, so a mask is required similar to those used for solder paste application.
The obvious way to create such a mask is with modified pads in the same way as for solder paste, but this has some major difficulties (see below), so in practice, it's better to use shapes. The biggest problem with shapes is that they are drawn using lines, so all corners will be radiused by half the line width in use. Normally that would be undesirable, but given the nature of glue, in this case it's beneficial, as it reduces the possibility of excess glue being trapped in the corners.
Setting up the glue layer
If you do not already use one, you will need to create a custom pcb technology file. Here's how.
Any technology file can be opened just like a design file, but it does mean browsing to the right folder. Here's an easier way. Go to [File], [Library] and select the 'PCB Symbols' tab. Click on the [Tech File] button near the bottom. The dialogue that opens has a pull down list of available technology files. Select the one you want as a seed file, click [Open] (which opens the technology file on a new tab in the background), then click on [Cancel] to reselect the original file and close the window.
When you close the library manager, you will see the selected technology file open on a new tab.
You will need to create a new layer type and matching layer for the glue information.
Go to [Settings], [Design Technology], and select the 'Layer Types' tabs. In the layer type dialogue, select [Add]. The new layer type needs an appropriate name (such as 'Glue'). All pad types should be disabled. Usage, of course, will be 'Non-Electrical'. Click on [OK], confirm the new layer type appears correctly, then click on [Apply].
Now move to the 'Layers' tab. Select [Add]. The new layer will need a name such as 'Top Glue' (or 'Bottom Glue' as required), the type will be 'Glue' or your equivalent, side will be 'Top' (or 'Bottom'), 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 use [File], [Save As] to save the modified technology file to a new name of your choice. Note that you will need to set it as the default for pcb symbol editing as described in the second paragraph in this section before opening any symbols for editing, or the new layer won't be present. If the design already exists, use [Settings], [Technology Files] to transfer the new settings from the saved technology file into the design.
Setting up the glue spots
Note: To avoid also editing components, it is possible to save the modified symbol to the same name as the original. However, this MUST be done to a custom library, or there is a very real risk that the changes will be lost if the original library is overwritten by an update. The custom library should be in it's own folder at the top of the search path to ensure that the modified footprints are used preferentially.
The line width/style used for the glue spot shapes determines the corner radius. As it's undesirable to have these corners too sharp, a minimum width of 0.1 mm or 0.004" is suggested. Wider line styles may be used, but the constraint then is how small the spot can be made when securing very small components.
For existing components, use the 'Edit symbol in Library' function, otherwise find the relevant symbol using the library manager or Databook (from the [File] menu) and open it in an editor. Use [Add], [Shape], [Rectangle] (or [Circle] if preferred) to create an arbitrary shape of approximately the right size in roughly the right place. Precision at this point is not important. When the shape has been positioned, press [OK], then right click on it and open the properties. Check the 'Filled' box, change the layer to the glue layer, then press [OK].
Set a relative origin at the centre of the symbol, then go to [View], [Dockable Bars] and select the 'Shape Information' bar. The shape should still be selected, so information about it will be displayed in the dockable bar. Choose 'Rectangle' (or 'Circle') as the display mode, then type in the correct figures for the size and position, using the 'Rel' check box to make the figures manageable. The shape will correct itself as you put in the modified figures. When you've finished making changes, click on any different cell to close the last edit.
Add any extra glue spots as required, then use [File], [Save to Library] to save the modified footprint to your custom library.
Why pads can't be used to define the mask
On the face of it, pads would be ideal as they're easily customisable and a regular shape. The problem is managing their scope. Single layer pads are allowed in a design, and they can also be valid for non-electrical layers. The problem is that adding the pads in a design is not enough. They must be added within the pcb symbols to guarantee accurate alignment. However, there's a constraint on pads in pcb symbols which prevents them being assigned to any but the notional layers [Top], [All], and [Bottom]. That makes them unusable, as any glue spot pads would also appear on at least some electrical layers.