This page is is part of my embedded system notes.

Solder Paste Stencil Notes

Introduction

This document contains some notes about obtaining and using solder paste stencils for prototyping.

Possibilities

The following possibilities come to mind:

Professional Etched Stencil
This is clearly a reasonable option for mass produced product. For personal prototyping it is a little pricey.
Laser Cut Stencil
Pololu provides a laser cut stencil service where they cut some mylar sheets:
http://www.pololu.com/catalog/product/446
At the time I write this it costs $21 + $2/in². If a bunch of stencils are bundled together this is fairly reasonable.
Milled Stencil
The following web site has a page on the process (see Making a SMD Solder Stencil)
http://millpcbs.com/index.php
It looks like it would work well for larger SMT stuff, but not for the fine pitch stuff. I could be wrong though. Obviously, a pretty good CNC set up is required.
Drilled Stencil
Rather than milling the stencil, it can be drilled. The following web site talks about this briefly:
http://www.groupdiy.com/index.php?topic=46382.0
This looks like it could work pretty well. It might even work with fine pitch stuff.
Comes the PCB
There is at least one PCB house that will provide a low cost stencil with the prototype PCB. As I write this, PCB Pool does this:
http://www.pcb-pool.com/

Solder Paste Machine
There are relatively low cost solder paste machines available on EBay. These machines can be mounted in a CNC and instructed to dispense solder under computer control. We actually tried this and here is a video:
http://youtu.be/Yg8YRLRvTS0
This worked pretty well for the coarser pitch SMT. The fine pitch stuff needs a finer needle. Unfortunately, the solder paste machine does not like to push paste through the finer needles. It might be possible to make this work, but it would take some more effort.
Home Etched Stencils
It is possible to etch a stencils at home. For this strategy, I am using presensitized material that is exposed using a contact print, developed, and then etched.

Home Etched Stencils

KiCAD Configuration

I use KiCAD for my schematic capture and printed circuit board design. KiCAD is open source software runs on multiple platforms with no artificial restrictions.

In order to generate the files needed for the phototool, it is necessary to do some configuration.

Under [Menus] => [Preferences] => [Dimensions], Set the {Pads Mask Clearance:] to some value. I use -0.003 inches.
I edit the Pads for the NPTH mechanical holes. First, enable the [SilkS_Front] on the Technical Layers. Next, it is necessary to edit the Solder Solder Paste Clearance to reduce the solder mask diameter to be just the diameter of the hole. This way the solder stencil will have a holes that line up with the mechanical holes.
I make sure the PCB edges have I width of .010 inches. This requires editing each line and resetting the width.
The fine pitch IC's may need to have a separate solder paste clearance set. This done by editing the footprint. For the .5mM pitch Quad Flat Packages, I use -0.001 inches.

There are multiple ways of plotting the Gerber (aka RS274X) files. I set everything up once so that it can be used for both the stencil and the PCB. To bring up the Plot dialog box, I use Menus => File => Plot.

Under Layers, I select [Front], [Back], [SoldP_Front], [SilkS_Front], [SilkS_Back], [Mask_Front], [Mask_Back], and [PCB_Edges].
Under Options, I only select "Plot module reference on silkscreen" and "Plot other module texts on silkscreen".
Under Gerber Options, I only select "Use proper filename extensions" and "Exclude PCB edge layer from other layers". I definitely do not click off "Subtract soldermask from slikscreen" since it currently causes problems with gerbmerge v1.8.

I click [Plot] and it generates all the Gerber files.

Phototool Preparation

The phototool is printed on a piece of transparency film. In order to increase the opacity to light, I actually cut out two of the transparencies, and lay them on top of one another. This requires that I generate two copies. The easy way to do that is to print two copies, but that wastes transparency film. Instead, I use gerbmerge to step and repeat a couple of copies.

The file below (called motor3.cfg is used to configure a PCB (called Motor3) for replication. Almost all comments were stripped out to make the file smaller.

[DEFAULT]
projdir = .
robusdir = %(projdir)s/../..
MergeOut = motor3

[Options]
CutlineLayers = None
CropMarkLayers = None
FabricationDrawingFile = %(mergeout)s.fab
ExcellonLeadingZeros = 0
OutlineLayerFile = %(mergeout)s_PCB_Outline.gbr
ScoringFile = %(mergeout)s.sco
# The stencil has to fit on an 8.5" x 11" mylar piece.
PanelWidth = 8.0
PanelHeight = 10.5
LeftMargin   = 0.1
RightMargin  = 0.1
TopMargin    = 0.1
BottomMargin = 0.1

# Set X/Y spacing to 0.5in
XSpacing = 0.5
YSpacing = 0.5
CutLineWidth = 0.01
CropMarkWidth = 0.01
AllowMissingLayers = 0
DrillClusterTolerance = 0
MinimumFeatureSize = *topsilk,0.008,*bottomsilk,0.008

[MergeOutputFiles]
Prefix = %(mergeout)s_etch

*TopPaste=%(prefix)s-SoldP_Front.gtp
Drills=%(prefix)s-GM.drl
BoardOutline=%(prefix)s-PCB_Edges.gbr
ToolList = toollist.%(prefix)s.drl
Placement = placement.%(prefix)s.txt

[Motor3]
Prefix=motor3
*TopPaste=%(prefix)s-SoldP_Front.gtp
Drills=%(prefix)s-GM.drl
BoardOutline=%(prefix)s-PCB_Edges.gbr

In addition, there is a definition file called motor3.def that looks as follows:

Row {
  Motor3
  Motor3
  Motor3
}
Row {
  Motor3
  Motor3
  Motor3
}

This makes a total of six copies of the solder paste mask and PCB edges. (Two rows of 3 each.) It is run as follows:

echo y | gerbmerge motor3.cfg motor3.def

The output shows up in two files called motor3_etch-PCB_Edges.gbr and motor3_etch-SoldP_Front.gtp.

Next, I use the gerbv program to view the step and repeated files. gerbv is part of the open source gEDA tools. I installed gerbv using:

sudo atp-get install gerbv
{Password typed in}

To view the two Gerber files, I do the following:

gerbv motor3_etch-*.g?? &

and gerbv is started and both Gerber files are shown.

The next step is to use gerbv to generate a .pdf file that contains the Gerber files. The following steps are performed:

I change the background color from black to white. Select [Menus] => [View] => [Change background color]. I change [Color name] from #000000 to #ffffff and click [OK]. The background should now be white.

#{whatever}

#000000

Using [Menus] => [File] => [Export] => [PDF ...], trigger a the [Export PDF file as...] dialog box. Type in the name of the file and click [Save]. In this example, I use motor3_etch.pdf.

We are not quite done yet. The output file from gerbv needs to be mirrored horizontally. The reason for this is because the etching process will etch down and out. The hole on the top of the stencil will be smaller than the one that etches through the bottom. It is recommended that the smaller hole be on top and the the larger hole next to the PCB during solder paste application. Thus, we need mirror the image.

I use a program called inkscape to do the mirroring. For me, I installed it as:

sudo apt-get install inkscape
{Type password here}

The program is run as follows:

inkscape motor3_etch.pdf &

This causes the inkscape to start up and show the solder paste image.

Using inkscape, the following is done.

Using the mouse, select all of the artwork. Right click on the upper left corner and drag the mouse to the lower right corner. Make sure that the region select box encloses everything.
Using [Menus] => [Object] => [Flip Horizontal], the everything is flipped horizontally.
Using [Menus] => [File] => [Save As...] to bring up the file save dialog box. Type in the new file name and click [Save]. In this example, I saved it as motor3_etch_flipped.pdf.

Now the artwork is ready to be printed.

First, a mirrored artwork is printed on a piece of paper. The paper is examined to make sure it looks right. I use some calipers to make sure the printer is not adjusting the size of the artwork. That is what the PCB edges are for.

If the paper copy looks good, I shove a transparency film into the printer and print again. Again, I use some calipers to verify that the dimensions have not been changed.

The next step is to cut the transparency up into solder mask pieces. I cut outside the PCB edges and leave enough space to tape outside the PCB edges.

Using a piece of glass from a picture frame, I tape the edges with electrical tape so I will not accidentally cut my finger handling the glass. The glass is cleaned using some glass cleaner. The first cut-out is attached to the bottom of the glass such that when it is examined through the top, it is in the mirrored configuration. Next, using a microscope I attach another cutout exactly on top of the previous one. Make sure both cut outs are complete flat with no bowing.

The phototool is now ready use.

Stencil Exposing, Developing, and Etching

{more goes here}