Tell me more ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.
up vote 4 down vote favorite
1

How close can I place two 0603 resistors on a PCB?

share|improve this question
2  
Are the resistors on the same signal (in series, end-to-end or parallel) or on different signals? – Kevin Vermeer Dec 15 '10 at 1:33

4 Answers

up vote 4 down vote accepted

I have a silk layer bounding box of 2.6mm x 1.4mm around the pads of 0603s, and I often place resistors with touching bounding boxes. Lengthwise placed next to each other this leaves 0.2mm between pads. For reflow soldering this has never caused problems. For wave soldering you will need more space, esp. in the wave direction. For hand soldering it depends on the soldering skills of the person who assembles the board. 0.2mm may be possible if you don't use too much solder.

While 0.2mm may look like very tight, remember that this is reflow soldering. When the solder paste melts it's capillarily drawn to the contact surfaces of the resistor, so it won't flow to adjacent pads.

share|improve this answer
up vote 3 down vote

If you need several resistors with the same value as close together as possible, use resistor arrays instead of individual parts. They save a lot of space.

share|improve this answer
2  
I think I got better than a 50% space savings per part by using 4x0402 arrays instead of discrete parts – Nick T Dec 15 '10 at 21:44
1  
The law of conservation of misery says that the other resistors with the same value are the completely other side of the board :-( (OT: stronger law than conservation of energy or momentum, BTW; another observation of this law is that every wire cut to measure is too short) – stevenvh Dec 16 '10 at 16:40
up vote 2 down vote

This can vary a lot.

Fab

How is it being soldered? By hand or pick and place? What fab house are you using? What are their requirements?

These are things you should ask yourself and get answers for in order to determine how close is possible for the fab process.

Signal Integrity

You will also need to look at what signals are on each resistor. When you have high speed lines you can have issues. Also if you have high voltage you can have issues.

I know this is rather broad. If you have a specific case I will be willing to add more.

share|improve this answer
2  
When you place a resistor down, you are effectively putting the wire a little higher above the ground plane. When you do it with two devices near each other you will get both devices having increased cross-sectional area next to each-other, but gaining inductance and a large portion a mutual inductance. This can hurt signal integrity a lot, as you will bounce the other traces signal. @kellenjb, just expanding on your signal integrity section a bit. – Kortuk♦ Dec 15 '10 at 0:24
up vote 2 down vote

From here "The document is "IPC-7351A Generic Requirements for Surface Mount Design and Land Pattern Standard". You have to buy it from www.ipc.org." You CAD package may have it already. There are 3 variantes, so you would use the "least" (i.e. smallest one).

"If you want to look at the recommended footprints, without buying the standard, you can download a free viewer at: http://landpatterns.ipc.org/default.asp

There's more info available at: http://www.ipc.org/ContentPage.aspx?pageid=4.6"

share|improve this answer
2  
Direct links: dis'vun and dis'vun. – tyblu Dec 15 '10 at 19:10
1  
Mentor Graphics' LP Wizard is IPC-compliant and has a 10-day trial. – tyblu Dec 15 '10 at 19:15

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.