[SOLVED] Altium Designer and SMT Stencil

Hi guys,
I'll be doing my first reflow soldering (bought a reflow oven) and I need to make a soldering stencil for my PCB. I am working in Altium designer 10. I have two questions:
- The pads in the Top Paste layer should be 10% smaller for the SMT stencil. How do you scale all pads in AD by 10% ? I can set the paste mask expansion rule to something like -0.05mm, but that's not 10% (obviously).
- How thick should be the solder stencil. Is the 0.12mm standard?

Thank you guys for helping out.
George

Hi George,

To my knowledge you can't specify a % value in the paste mask rules... (This has been requested). You can however set an expansion rule for every component in you library. This way you'll get something close to what you are after.

Hope this helps,
Chris.

Now that's a neat Idea that I haven't thaught of, and it would work, but there's a problem. If I decide to make several boards and ship the files to a manufacturer, the Paste layer must be 1:1 with the pads (ie expansions set to 0). If I modify the expansions in the library for each component, than that would make the libraries useless for series production. Modifying each part individually in every PCB design... no go, especially if you have like 200 resistors on the boards

Any other ideas?

George

Yeah that is the downside... and moding the libs every time really isn't an option.

You could in theory do it in the rules for every design but you'd still need to do it for every footprint - i.e has footprint 0603 -0.05mm as some rough syntax.

Unfortunetly I can't think of an elegant easy way to do this. Hopefuly someone will have another idea.

Chris.

I might not be able to give you exact procedure but you cantry out this option.
You can do that through PCB list tab.
In that TAB you have to make paste mask column visible (remember to select smd pads only, this will make it easy).
Now copy that column to excel file (now you have to know a bit of excel for this) set a new column in excel to set the rule for 10% reduction of the value.
You can copy back this reduced value to altium PCB list, remember to maintain the order and manuly verify once.

Hope this might help you or give you some idea.
Best of Luck

you could add a layer into your library which will be used to make your own stencil.

Do all stencil artwork 1:1
There is a wealth of information regarding solder paste stencils on the web, I would reccomend you study it as stecil design and problems accounts for over 60% of the faults found on an SMD line. It is critical to making the product, use 1:1 and work with a good stecil manufacturer.
Dont alter the pads in your libaray, how will you cater for different thickness of stencils etc...
Printed Circuit Design and Fabrication has numerous article on stencils.

---------- Post added at 12:26 ---------- Previous post was at 12:21 ----------

Tecan - SMT Stencil Products
**broken link removed**

OK, I've found the sollution:
1. Use soldermask expansions set to 0 in PCB
2. In CamTastic, when generating gerbers, there is a "scale" tool, which allows to to scale any object in %. So select the paste layer and scale all pads by 10%.

So voila. You can't do scaling in the PCB, but you can do it in the gerber editor.

Thanks to all for you input!

Curious as to how a figure of 10% was reached?
The important figure is volume of paste required for each component, and this depends on the solderpaste screen thickness, even more complexif you use multi-thickness screens.

I am trying to reduce the surface of the pads of a micro controller on the stencil by 10-13%, in order to avoid excessive solder that could couse bridges. I have tried changing solder mask expansion value of the pads to 0 in the PCB, and then tried scaling in camtastic (from edit--objects--scale). However, when I do that, a box shows up and ask a scale factor to type in and does not accept negative values. Just to see what happens, I typed 10 and did not wish to scale the apertures. At the end, all the pads I choosed becomes a single thick pad.

Is there any other way of scaling the size of the pads of an MC ?

Thanks

Does this scaling only shrink the PADs or it shrink the whole board ? If it shrinks the whole board, the position of the components will also be changed... am I right ?

- - - Updated - - -

Mercury said:

OK, I've found the sollution:
1. Use soldermask expansions set to 0 in PCB
2. In CamTastic, when generating gerbers, there is a "scale" tool, which allows to to scale any object in %. So select the paste layer and scale all pads by 10%.

So voila. You can't do scaling in the PCB, but you can do it in the gerber editor.

Thanks to all for you input!

Click to expand...

I do designs for several large aerospace companies and they require 1:1 for the solder paste layer in the design files I deliver. To support this the component libraries must be 1:1. The reason for this is they up load the Gerbers to an assembly shop that will then order the PCBs and stencil. The assembly shop will scale the solder paste Gerber to match their specific processes for solder paste printing and then order the stencil. Each shop has their own scale to match the paste they buy, their preferred stencil thickness, and their paste printer.

I assemble the first prototype PCBs and therefore order the stencil. I scale the paste using the Rules by setting various scales by classes. As an example 0402s are a class and are scaled by -5mils x -5mils. Occasionally, I have left it to the stencil shop (e.g. ASI Stencil Associates) to apply their "standard" scale factor with good results so far.