We always have in our designs situations where one pin of a row of SMD discretes (mostly 0201's) is tied to a solid plane of copper with no thermals. Over the years, our fab houses flag this and have requested to adjust the mask opening on the plane connection to make it smaller so that it doesn't become a larger 'pad' than the other side of the discrete. We've had this done this successfully over the years. The question has arisen whether we could make this adjustment ourselves within Allegro so that the fab house doesn't have to do it. I can't think of a quick and easy way to do this. How does everyone else accomplish this? Thanks for any insight you can offer.
HI, there is not a good way to do this dynamically. You could create a soldermask that is 1:1 with the pad and let the board house grow the mask at the gerber level. This will give the board house some latitude. Dependingon the soldermask the boardhouse uses they should be able to get withing +/- 2Mils of the pad. On something like a 0201 i use round pads for the footprint with a soldermask that is + 2 mils over size of the pad.
From your post it seems the fab house are running into issues with the solder stencil. They may have a concern with solder bridging, not too sure. If you can post a pic of the 0201's hitting the plane I may be able to offer you a little more advice
All the best.
Thanks excellon1. There hasn't been a problem since the fab house has been asking if they can reduce the soldermask opening on the pads encapulated by planes, and I always say yes. However, management is asking if we can avoid having the fab house make any soldermask changes, so therein lies the problem. I can't figure a way to do this at the layout level. Looking for other folks' experiences with this. Thanks.
Thermally relieve the discretes, so that the GND pads actually show. (e.g. tie the pads to GND with a large copper trace, essentially 'pouring' them as you've done historically) That way the fab shop sees a pad on each side of the discrete and opens the soldermask equally on both sides. Your problem should go away, with little changes to your process. Thermally relieving the GND pad should not affect any performance.
We have a very similar issue and on small parts such as 020s1 it can create an assembly issue since each side has a different metal exposure. Even just switching to a thermaled connection does not solve the metal exposure issue since the extra metal from the thermals bleeds off solder unevenly. I suspect these are caps since you want to reduce any possible extra inductance? If they were resistors that were pullups it makes sense to connect with a small trace and not direct connect to the plane. To deal with this we have an alternate part with soldermask defined pads. When placing you can right_mouse->alternate part assuming you set up the alternate footprint in OrCAD or Concept (DEHDL).
You can also do just an instance replace of the pad attached to the plane after initial layout is done. You would have to replace the pad with a soldermask defined pad. I find that a bit error prone.
...Except when doing RF layout where thermals add a small parasitic to the C or L. For LF work its OK, but for RF/uWave it may not be a good idea.