Note: You must be registered in order to post a reply. To register, click here. Registration is FREE!
T O P I C R E V I E W
georg.schmidt
Posted - 25 Mar 2014 : 07:01:42 Hi,
sometimes it is necessary to apply vias in pads, e.g. for thermal pads. Is it possible to apply such vias without getting a "Via in pad"-error in the design rule check?
Regards, Georg
3 L A T E S T R E P L I E S (Newest First)
steve
Posted - 26 Mar 2014 : 09:35:23 I would suggest that the key to the question is that the copper and vias that you wish to be associated with each other but do not want them to cause DRC errors is simply to assign them each a simple common net name (not the future one in the design, just one you think of) within the footprint. If then in the design you wanted to strap the copper to say GND, the copper and the vias will adopt that signal name.
Pulsonix Assistance
jameshead
Posted - 26 Mar 2014 : 08:58:27 You will always get a DRC error if you've got the "Via In Pad" check turned on, if the via is on the same net as the pad or not. The "Via In Pad" check is under the "Nets" section and may not be turned on by default.
It's a useful check to make sure that vias aren't too close to SMT pads so as to cause solder theiving during reflow.
As Ben says you can add the vias to the footprint and turn off the DRC checking in a footprint if you don't want to see them, however I wouldn't advise doing this.
It's far better to have them come up as errors occasionally and then lock them to indicate you've seen them and that they are okay.
Alternatively you can draw an area around the thermal pad, name the area "thermalpad" for example, then in Set Up Technology use Match Net Class Pair and set up a rule for Ground to Ground net class within Area "thermalpad" and make the Via to Pad spacing minimum spacing 0.00 but this is far too much hassle I would have thought compared to just locking an error.
bkamen
Posted - 25 Mar 2014 : 17:04:03 Could you be more specific?
I put via's inside QFN/DFN footprints all the time for excess solder channeling as well as heat dissipation and I don't get those errors.
(They are part of the same NET)
There's also a setting when creating footprints to not generate errors for items inside a footprint. (I'll have to go find it again) which could be part of your problem.
