No announcement yet.

footprints for an 0603 resistor from three different vendors

  • Filter
  • Time
  • Show
Clear All
new posts

  • footprints for an 0603 resistor from three different vendors

    Hi Robert,

    I am trying to build a single footprint which could be used for three different manufacturers of a 1K 0603 resistor (Yageo - RC0603FR-071KL, Panasonic- ERJ-3EKF1001V, and Vishay- CRCW06031K00FKEA). I looked up the data sheet for all three and used the dimensions from those data sheets to create three different footprints using Altium Designers IPC Footprint Wizard (I am using the latest version of AD, 21.3.1). The Vishay data sheet had a recommended footprint for a reflow process which was quite a bit different than the other three. I have attached a snap-shot of all four of those footprints which I created in Altium.

    Even though all three of these components are approximately the same size (1.6x0.8mm), the three IPC footprints were all a little bit different. However, the Vishay recommended footprint was quite a bit different.

    What are your thoughts? How would you approach this problem of creating a footprint which would work on all three?
    Click image for larger version

Name:	four 1K footprints.JPG
Views:	6026
Size:	48.4 KB
ID:	17291

  • #2
    Different solder flows and different manufacturers recommend different pad dimensions. For an 0603 resistor, it probably isn't hypercritical, but the larger the pad, the higher the capacitance, so for high frequency this makes a difference. 0603 isn't really a good high frequency resistor, so probably not an issue.

    In a similar way, longer and narrower pads increase the series inductance in ceramic capacitors, reducing the effectiveness of the capacitor for high frequency decoupling and possibly required additional capacitors to compensate. The wider bands create a narrower path and connecting the traces to the insides of the pads reduce the inductance of the capacitor, improving the decoupling effectiveness.

    I have a paper on the topic of partial inductance (the capacitor ESL effect) at EDICON in August and I will show the measurements of the components and how the pads impact the partial inductance..

    In the meantime, discuss this with your PCB manufacturer and/or the component vendor to determine the best footprint. I often use the larger dimensions for lower frequency prototype work, since it allows me to hand solder or to use automatic soldering and I'm not wording about the life of the board. For higher reliability and/or high frequency projects that isn't a good idea.


    • #3
      Ultimately, unless you care about frequency, capacitance, and having to implement anti-pads, it's going to come down to what your assembler is comfortable with. I would work with them.
      The last footprint in your screenshot looks like it would be great for high-frequency terminations, but my gut feeling is that it's bad for manufacturing. At that pad size, I'd be changing to an 0402 to avoid having reflow problems. In saying that though, I don't claim to be an expert on reflow and tend to depend on my assemblers.

      In case it matters, I use Altiums IPC wizard for small chip passives with medium density courtyard settings and autogenerated pads unless I have a very good reason not to (maybe I'd use high density in some cases). Medium density is good for rework even on 0402 sizes without compromising too much on PCB realestate.


      • #4
        I usually go with the middle way. We only use super small footprints in high density designs or under BGA where they have to fit between pads. We use bigger footprints if we know the components may need to be hand soldered.


        • #5
          Hi to all,

          Please check Same chip size but different terminal metalization - PCB Libraries Forum

          I asked myself the same not a lot of time ago.

          I hope you find it useful.


          • #6
            Thank you for those responses!

            Here is another footprint I have been struggling with, an 0402 capacitor. The part number is "LMK105C6105MV-F" from Taiyo Yuden. It's spec shows 1.0+/-0.05mm for length, 0.5+/-0.05mm for width, and 0.25+/-0.10mm for the terminal metallization. I put those numbers into the IPC Footprint Wizard and got the footprint shown below. I then drew a projection of the component on the footprint. In order to make sure the entire terminal is on the pad, I used the max dimensions for width and terminal metallization, but I used the minimum dimension for length. As you can see in the attached image, it looks like the terminal just barely fits on the pad. So assuming the goal is to get the terminal completely on the pad, the footprint generated by the wizard looks good.

            However, as you can also see from the image, there is only 0.22mm between the pads. 0.3mm would be needed to support a 0.1mm solder mask expansion and a 0.1mm solder mask dam between the two pads (0.1+0.1+0.1).

            I could make the pads a little smaller (to make more space between them), but then the worst case terminal would not be completely over the pad. Maybe the better approach would be to use a 0.05mm solder mask expansion which would leave a little over 0.1mm for the solder mask dam. Which approach is better?

            Click image for larger version

Name:	0402 cap.JPG
Views:	3122
Size:	58.7 KB
ID:	17377


            • #7
              I can't judge the footprint much but I think your spacing is within the capabilities of most fabricators.
              Where did you get 0.1mm from? I think the unofficial industry standard these days is 2mil (0.0508mm) expansion and 4mil (0.1016mm) sliver/clearance. That's a total of 8mil (0.2032mm) which is within the 0.22mm spacing of your footprint.

              The are other things to consider though. Fast turnaround or cheap fabricators might want more expansion but I don't really know. Even cheap fabricators like Elecrow, AllPCB and PCBWay operate on those numbers.
              Epoxy filled/capped vias will affect microstrip clearance but I'm not sure about solder mask.
              Last edited by DanR; 05-03-2021, 03:35 AM.


              • #8
                Dear Tom,

                I created the component using PCBLibrary Expert. It is a program from where I am learning a lot about footprints; the forum is from where I learning more.
                They have a very useful free pad calculator. It is based on IPC-7351

                Robert made a video with them, very very interesting. Here it is.

                Using that program the distance between the pads is 0.34mm.

                How do you created your footprint?
                I attached the mentioned footprint.

                I hope it will help you.