I have to create an SMA connector library, but i didn't find proper dimension in data sheet and even net. Attached the image of SMA connector and what might be the dimension of A,B and C? And also the trace width? I think B is 4mm and 1.1mm and 2.2mm holes are Plated TH.Any input will be appreciated.
I would call the manufacuter tech support for the part and ask them for the recommended land patter for the part. I have had to do this on multiple occasions when the data sheet wasn't sufficient.
In reply to KEN13:
Thanks KEN for your kind reply.
In reply to C Shiva:
Not all manufacturer offers free footprints. To many, maintaining a library
of such is difficult. For instance, handeling the solder mask openings vs copper surfaces
differs from region to region. There is always a risk that you will end up trusting a footprint that
you yourself did not create according to your companys specifications.
I regularly create footprints of simple and more complex connectors, and what I look for
besides drawings and dimensions are .DXF-files. I am not endorsing any company ove another, but for instance
Tyco has a very good library of both datasheets and .DXF's.
1. I download the drawing, and use the create footprint wizard in PCB-Editor in order to create
the connector pins and the mounting holes. In almost all cases, there are quite a bit of manual
calculations that has to be done, since mech guys simply do not use how to apply dimensions to a footprint.
While the connector pins can be easily defined, the mounting holes always has to be added manually
and here you have a choise wether to make them mechanical or electrical. Making them mechanical will not
enable you to attach them to a net, which is important in case of ESD-requirement (if the body is of metal
2. I then delete the automatically created outline (ASSY / SILK) and instead use the downloaded .DXF...
3. Open the .DXF in a mechanical CAD program (such as AutoCAD Lite). Edit the drawing
and/or scale it to the same unit of measure used in the PCB Editor. PURGE unneccesary/unused layers.
3. Open the newly created footprint in the PCB Editor, and choose Import | DXF. Make an INCREMENTAL (!) Addition and map the .DXF layers to the ones that you want (ASSY / SILK). (takes a bit of training but this is well worth it!)
4. Proceed with Import and note that the outline ends up somewhere really outside the drawing extent (Hey Cadence: This is a bug in the PCB Editor - It does not matter if the UCS/Zero is correctly set using the Mechanical CAD or not).
5. By properly choosing entities, now move the outline to its correct location using keyboard entry or simply by
enlarging the drawing enough to minimize optical error.
After importing the outline, modifying the DFA_Bound and PLACE_Bound is very simple.