What is everyone using to calculate paste stencil artwork?

It is relatively simple to create Skill code that decrements paste pads (that are not pre-decremented in the library). My company uses a decrement of 50um (25 each side) as a global rule of thumb. This creates shapes on a Manufacturing/Pastemask layer which is then used for the film. The trick is to then verify the area ratio and volumes to ensure that these new shape meet your DFM guidelines.

The Allrgro Productivity Toolbox has a Mask Generator that will do this for you. For info look at  <your_install_dir>\share\pcb\toolbox\help there is a genmask.pdf that describes the process.

Just fyi that Allegro X already introduced a subtle feature to help with paste and soldermask pad creation. I think it's really useful but there was not much fuss made of it. 

Just use the right mouse button and enter the increment or decrement gap to the pad layer.... (see image) 

So no need to check the pad dims on the design layer tab, just tell the expansion values to the tool. 

First rmb menu looks like this:

Subsequent menus look as follows:

Just fyi the assembler will likely choose a specific stencil thickness depending on their production setup such as paste type choices, or design specific reasons such as minimum component pitches, min pads sizes, versus and large paste deposits needed for large power components.( just as example). Therefore they will typically adjust the "area" of all paste deposits on the board to counter the change in stencil and to rebalance the actual "volume" of paste put down. Some of the discrete paste deposits may even be adjusted with special "v" shapes or other tricks; an example is "home base" stencil opening shape which is pretty common for caps and resistors.... 

From my experience it is more important to adjust copper pad length/width as problems with soldering can start there, which may not be possible to fix by adjusting the paste shape alone. 

Would love to hear any other experiences of designers in the field; or any other questions. 

Hi John,

That looks to be a nice addition to the Padstack Editor, kind of similar to shape expansion, contraction in the PCB editor, cool stuff !

I echo your thinking on adjusting the land pattern in that if it is not optimal then soldering issues can occur. On a PCB that uses regular
rectangular pads for the SMD pads components more often than not if one inspects the board they may notice that the physical solder
paste does not cover the whole pad. Typically the corner area do not have paste.

A better approach is to use rounded style pads instead. This aids in the release of the solder paste screen and will allow full utilization of the pad from the paste perspective. There are kind of two camps on this. The first is I don't care as long as the part is soldered down :)

The second stems from how a stencil is cut. Its very hard to have a laser do right angles, so why go that road to begin with. Knowing this it is better to design the land pattern with that in mind.

Best regards.

Really good tips excellon - totally agree!