6 Replies Latest reply on Jan 10, 2018 7:20 AM by tarribred61

    Footprint Origin for Pick and Place

    jimku

      My questions have to do with part footprint creation and pick and place files. When creating a new footprint, should I be concerned with where I place the origin such as at pin 1 or the centroid of the part? For example, on a 2-pin part, should the footprint be horizontal or vertical? If horizontal should pin 1 be on the left or right? If vertical, should pin 1 be up or down? I have similar questions on multi-pin components but do these types of questions matter? I recently had a board made where the assembly house wanted the pick and place file and I gave them what CircuitStudio generated and they had no questions and got it all correct. This project was a board imported from PADs with a few changes that I implemented. I looked at the file and noticed that the Pick and Place file shows the Mid-coordinates matches the Ref-coordinates for the components that I generated the footprints for, but the components that stayed the same shows the Mid-coordinates matches the Pad-coordinates.

       

      Is there any information describing where the origin should be placed and what orientation to use when creating a new footprint?

        • Re: Footprint Origin for Pick and Place
          e14softwareuk

          In my experience it doesn't really matter because there is always manual setting up of the machine so any reasonable data from the CAD system should be good enough. Traditionally I have always had the reference point of library items as pin 1, typically with pin 1 drawn upper left unless something different makes sense.

            • Re: Footprint Origin for Pick and Place
              tarribred61

              I think the industry standard for ICs and passives is to locate the centroid in the body center of the device where possible.  For asymmetric footprints (e.g. some connectors) it can be the body or pin 1.

               

              I have an older circa 2009 version of the IPC land pattern calculator from PCB Matrix that I find useful for checking footprints that I generate.  They were bought by Mentor Graphics and the tool may not be available (or for free) anymore.

               

              The IPC web site has a link to something that looks like it might be what I have and here is the link.

              IPC-7351 Land Pattern Calculator and Tools | IPC

               

              The older version might be available on-line but I can't say if the links I find with Google are legit and safe.

              1 of 1 people found this helpful
            • Re: Footprint Origin for Pick and Place
              e14softwareuk

              With regards to setting a reference point in the library, I would recommend making sure it is located on a pin otherwise you will end up with off grid components when creating a PCB. The reference point is the position the component 'hangs off the cursor' when adding or moving so if this is not aligned to a pin then the component pins will be off grid. I've added some documentation to cover the various fields in the pick and place file because it can be a little confusing to know the difference between the Mid, Ref and Pad locations.

              Pick and Place Data Format

              1 of 1 people found this helpful
              • Re: Footprint Origin for Pick and Place
                rajeshmau

                To decide the origin of any SMT components you have to refer its datasheet. The datasheet clearly mentioned the center of the components in its Tape / Reel information. Majority of datasheets also explains that the in which position the components will come in reel. According to its position you have to decide the orientation angle.

                 

                -Rajesh

                1 of 1 people found this helpful
                  • Re: Footprint Origin for Pick and Place
                    tarribred61

                    I agree with referring to the manufacturer's data sheet.  Also, good to keep in mind that while manufacturers often have recommended footprint patterns, they are often compromises and don't consider the various option of least, most and normal solder amounts that a designer may want to consider based on application and soldering method.  For those, not experienced with this, the basic idea is that the footprint might have a larger exposed pad if the part will be wavesoldered (including selective wave) versus reflow soldered versus hand soldered on the bench.  Often, to me at least, the tiniest parts such as EIA0402 and smaller need to use the smaller versions of footprints for reflow soldering or they tend to skew and tombstone as the melted solder paste hardens and surface tension acts on the joints. Of course, if you plan to prototype and hand solder then you want to have a more generous exposed pad.  These are some of the reasons it is not so simple to just find and download a one-size-fits-all footprint that someone else created.

                     

                    Another consideration is that in addition to the centroid location, it is essential to have a clear orientation marking in the footprint.  If the design is not high density, then this can be done in the legend/silkscreen layers.  However, if there is not enough space for silkscreen for every component then use of another two mechanical layers for a top and bottom assembly drawings is essential.  These can show the component body outline, reference designator and pin 1 location.  Where possible, a visible pin 1 (or cap polarity, diode bar, etc) mark on legend/silkscreen is useful for post-assembly inspection so it is best not to put the pin 1 mark under the chip where you cannot see it after the part is installed.

                     

                    It is also helpful to look on the internet or contact your assembler about design for manufacturing guidelines including their recommendations for common footprints.  Read the prior blogs on Sierra Circuits and other sites.

                     

                    A couple of links below:

                     

                    What Should My PCB Footprints Include?

                     

                    https://www.protoexpress.com/blog/becoming-a-pcb-master-design-for-assembly/