Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

[SOLVED] Pastemask. Manufacturing PCBs - PCB Editor

Not open for further replies.


Member level 2
Jun 12, 2009
Reaction score
Trophy points
Activity points
Hi all,

after finishing some designs, it is time to manufacture and assemble them.

For making these designs I have to create all padstacks, footprints, etc from scratch, so I took PCB Editor examples as guide for doing mine.
Now, when I send the gerbers (etch layers, soldermask, silkscreen, drill) to our manufacturing house, they requested me the pastemask ones.
Although they can generate them from gerbers, they are enquiring me to generate the pastemask gerbers with our own requirements.
So, I need a little help to get the proper guidelines to avoid any possible error.

Then, I wonder if you can provide some guidelines about how to define and create the proper pastemask layers.

From PCB Editor examples, most of passive components have no pastemask defined (SMT and THR), and from IC pads the relation between pads size and solder paste are 1:1 in most cases.

I have in mind next possible requirements:
  • THR components: 1:1
  • SMT components with padstack larger than 1mm: 1:1
  • SMT components with padstack shorter than 1mm: 1:0.9
  • IC perimeter pads: 1:1
  • QFN perimeter pads: 1:0.9
  • QFN thermpad: <1:0.7
  • BGA pads: 1:0.9
  • Any other pads: suggestions accepted
Are these requirements right?

  1. Which is the best option, provide pastemask layer to manufacturers? Or should I let him create them?
  2. In the case, I have to create the pastemask layers, which are the best guidelines to follow them?

Kind Regards.

All smt components 1:1
All PTH components - zero size

Any reductions can be done by the paste screen manufacturer.
If you want to define the reductions yourself you also need to do this with the thickness of the screen in mind.

I used to produce them at 1:1 and ask Tecan to adjust specific size apertures with x reduction - that way I could then send the same data to get another screen with different values is assembly decided that what they had was not right.
  • Like
Reactions: yolco


    Points: 2
    Helpful Answer Positive Rating
Stencils are usually ordered by the assembly house, they'll decide about stencil thickness and should prompt a paste pad adjustment when necessary, or if preferred, arrange it with the PCB designer.

In case of doubt, paste pads are 1:1, except for large pads that should be divided into small squares or similar.

Did you actually mean THR (reflow soldered through plated components) or plain THT?

If you are working with a recent layout tool, I would expect that you are using 80 or 90 % of tool vendor supplied component footprints (including paste pads) and redefine or make from the scratch 10 or 20 %.
  • Like
Reactions: yolco


    Points: 2
    Helpful Answer Positive Rating
Accually, PCB manufacturers could do the pastemask for stencil production themselves. Other stencil requirements could be noted to the stencil manufacturer.
As experience, for the SMT parts, you could make the pads a little bit bigger or longer for easier assembly if necessary, usually 1:1 should be the right choice. For the THT parts, it should be no need to make on the pastemask.
  • Like
Reactions: yolco


    Points: 2
    Helpful Answer Positive Rating
Thanks all!!

To sum up from answers and readings:

  • SMT components: 1:1 (included BGAs)
  • SMT Thermpad (ICs): 1:'x', read datasheet for 'x' recommended value.
  • THR components: 0, no need of pastemask for through hole components.

Then, in case of need to provide a specific apertures size, stencil manufacturers should be asked about the thickness of the stencil.

  • Aspect Ratio = W/T (Recommended >1.5)
  • Area Ratio = [(L*W) / (2*(L+W)*T)]
    • W - Aperture Width
    • L - Aperture Length
    • T - Stencil Thickness


Make ALL pads 1:1 in your library DO NOT ADJUST, that is the job of the assembly house in collusion with their stencil manufacturer... The most important factor is VOLUME of solder paste placed on a pad... There are many other factors (such as solder paste ball size), but volume is the critical one.. and when you start to use stepped silk screens the 1:1 is even more critical.
IPC-7093 for thermal pad guidelines.
IPC-7525A for stencil design guides, plus look for guides from the likes of DEK and Tecan.
If you are not assembling the board then you cant finalise the stencil design, 60% of reflow errors are down to bad paste printing and stencil problems.....

Not open for further replies.

Part and Inventory Search

Welcome to