I am working on a design which includes TO220 and SOT223 transistors.
Doing visual inspection, I noticed that the SOT223 SMT pin partially overlayed the TO220 through-hole. But I got no DRC error or warning about this. The pins ARE supposed to be connected (so there was not a short) but there was physical interference between the pins of the two devices.
Why no DRC warning or error?
When I made my own footprints, I included no courtyard. I was thinking that a pin collision such as I described would be an error worse than many courtyard violations (sort of like a real collision versus a near-collision in transportation) so that I should get an error or warning regardless of courtyard. But maybe my assumption is false?
Disclaimer, I don’t know.
But intuitively, this would seem correct to me, that’s what courtyards are for?
A possible use case that comes to mind is overlapping DNP resistors so I could configure either 1-2 or 2-3.
Thanks. Do you ignore the DRC warning about the courtyards interfering? Or do you drop the courtyards in custom footprints?
I am already doing that sort of thing…but I do it in my custom footprint. (I simplified in my OP above.) That footprint combines a SOT23 and SOT223 and 1206 resistor (use one of the three).
My thinking was that to do that, well, I am repeating my OP…
I did a board with a shaft encoder driving an up-down digipot. I really wanted to get the shaft rotation direction correct but was unsure based on the datasheets of the two devices. So I did (is it a crosspoint?) which takes two 0603 resistors. They can go 1-2 and 3-4, or they can go 1-4 and 2-3.
Thanks. Do you ignore the DRC warning about the courtyards interfering?
I haven’t done this with KiCad myself but it’s a fairly common design pattern, to configure boards during assembly with 0-ohms resistors.
I’d probably try making a copy of the resistor footprint with adjusted (or omitted) courtyard. Then see what happens…
Why would there be an error if pads of the same number run into each other? All you are making is a odd shaped pad, intentionally or not. As for the courtyard you should make one that encloses all the pads. That’s the disadvanage of a union footprint, the courtyard may be larger than needed.
Why are you still running a RC when the release is out? Though that’s unlikely to affect anything.
In different threads I have discussed a couple of related but opposite topics. So perhaps that is the cause of some confusion.
In this thread I am discussing two footprints with which (in my PCB editing) I have accidentally caused the pins to collide or overlay. I want to place BOTH devices. But alas without maybe going into quantum mechanics (or Australia? ) I do not know how to put two objects in the same place at the same time.
I had another thread:
where I discussed a combi symbol and combi footprint in which any ONE of three actual devices could be placed. That footprint is one half of the problem in this thread. The issue here is that my combi SOT223 collector has collided (my mistake) with the pin of a TO220 (separate footprint) and I saw no resulting DRC error.
As for 8.09 the last time I looked I did not see it without the “RC.” I had seen a post which recommended it. Right now I want to hold off from updating to 9.X.
You are confusing matters by calling them pins. In a footprint there are no pins, only pads.
If you are going to use only one part then you must create a courtyard for the new footprint. Pads on their own do not come with courtyards.
If you do want to put more than one part on the footprint why not just use separate footprints? Otherwise do not remove the individual courtyards when building your combo footprint.
Release Candidate. Thus 8.0.9 is the release following the 8.0.9RCs
OK sorry… But are you really going to call the TO220 pin (on the transistor) a “pad”? That gets to the “meat” of the physical interference problem.
Two reasons:
It makes re-use easier. In the case at hand, I am using four of them. Given the way I do things, it seems likely I may want to do it in the future. This way I do not need to figure it out again.
I was pretty sure that putting two pads in the same place (in PCB editor) would give me a DRC error. Doesn’t it sound like an error? Gosh I get DRC warnings for having a silkscreen run over a pad. Given the fact that the result usually is not a problem, that is much more benign than putting two device pads in the same place.
Nope. You only get an error if the pin numbers differ in the same footprint. And I think it’s the footprint editor that will call this out. If in the PCB editor then it’s the courtyard that’s supposed to catch this.
How does that make sense? Having the same pin number does not prevent physical interference. I am talking about two devices.
Yeah OK courtyard…I did not have one. But if you think about courtyards and hand assembly, it is easy to imagine (for example) two SOT23s where pin 3 of one device would touch into the plastic body of the other. It might not be so difficult to assemble, especially if you do the correct one first. But it would be a courtyard violation DRC error. On the other hand, co-locating pin 3 of a TO220 with pin 3 of a SOT23 would not be do-able (for assembly) but without courtyards you get no DRC error.
Courtyards are not perfect. They tend to be conservative. I have once ignored a courtyard clash between a THT resistor and the corner of a DIP IC because I know the resistor lead will not clash with the IC body.
It all comes back to your assumption in your first post. It is wrong. You might or might not get a net conflict error. The reliable way to catch physical clashes is the courtyard.
Oh, and any violation can be waived with good reason / choosing the smaller evil.
Note “exclude with comment” in DRC, awesome feature which I think is new:
