I'm new to OrCAD and have only done one design so far but I'm trying to figure out how to stick vias into a thermal pad. I have a QFN design from a friend and I can't tell if he did it as well but I've seen the board it created and he's got tented vias in the thermal pad and I can see from the design files that he's got the solder mask in a pattern and paste mask in a pattern so there's a clear place where the vias go but I don't see them on the package when I open it for edit. Is there a way to do this or is it done when you're creating the board or was it somehow included into the package pin but I'm not seeing it when I open up the padstack editor?
You can add the vias at the package level by using "add connect" in the menu. You will need a padstack for the large thermal pad and then you can add as vias as you desire to it. Be sure to add the padstack under the part as a pin in the component so that it shows up in the schematic. You are allowed to add shapes and vias under a part and connect them free-hand to any net if you want to but it usually is more cumbersome and results in missed connections in the final product. Ask more questions if you are still having trouble getting this right.
Thanks redwire - one other question; there seems to bee an auto keepout that's preventing me from putting it in the pad; is there a layer within the padstack I need to delete? Or somehow assign the net of the pin (in this case pin 101? since it's a QFN-100 and it's the 101-st pin) to let it go? Sorry - still new to this so I'm not sure how to manually override a keepout or turn off/accept the DRC errors
I am assuming you have added the desired via to the constraint manager physical tab so it can be used? When adding the connection you need to make sure the find filter has pins, shapes, and whatever else you want to detect on checked. You should be able to route from any arbitrary object and drop a via. If you are getting DRCs that's normal (another topic tho...). If you are getting some other DRC that is preventing the via to touch the pin then drop it and move it with "allow DRC" and hug/shove turned off.
If still stuck you can either post up the symbol here or PM it for a look. Or even a screen shot of what's happening.
Hi, for a ground pad on a QFN package what I like to do is create a padstack for the bonding pad and then use the multi drill function in the padstack editor to add as many drill holes to the pad as you want. The advantage is you don't have to add vias to the physical part to get the drill holes in the padstack. From a schematic perspective you are dealing with one pin even though you have multiple drill holes in that pad. As red pointed out you can also add vias etc. Here are a couple of pics to give you an idea. The first picture shows a rectangle pad in the layers section of the padstack editor. (16.6)
The second pic shows how to add the drill holes from the parameters tab.
You can stagger drill holes if you wish too. There is a wide latitude to customize the number of drills and spacing etc. Main benefit is that you are just basically dealing with one pad.
All the best
Sorry been doing other things but now that I'm back to this, I tried both ways and it looks like the drills get added to the part but the design doesn't seem to respect them as vias:
They're there but it only shows that it's a hole in my board and not that it's a via with a net associated (to the pin) and whatnot. Both ways that were mentioned by redwire and excellon1 worked though to put the part in, I just needed to tweak what I'm doing to put it into the pad/part. Thanks!