Stats

  • Locked Locked
  • Replies 4
  • Subscribers 165
  • Views 16429
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

IPC 356 A output error when working in metric

tmd63

Trying to generate IPC 356 A output keeps throwing errors and failing when we use D2PAK devices and the designs are in 'mm'.

The D2PAK device has a 10.5mm pad and this causes an error saying the integer value is too large '10500'.

Does anyone have a solution for the error? This error does not appear when the designs are being produced in imperial (mils), only when in metric (mm).

Any solutions please!

  • steve
    It's a limitation of the IPC standard and not the tools. There are only 4 columns 64-67 to write the information. Can't write 10500 into 4 columns. As the IPC netlist only needs a point and not the actual pad size you can either ignore this error or re-design your pad to be smaller and then use manually drawn copper in the filename.dra file to make up the additional size. If you do this don't forget to add the Soldermask and solderpaste shapes as well.
  • tmd63
    Thanks Steve,
    I would like to ignore the error, but I need the IPC file and the following pick and place files, neither of which will be created when this error occurs as it stops further operations in our automated output generation "Draft Center".
  • tmd63
    Ok. In OrCAD I could place a pad and then overplace a copper rectangle on the footprint to enlarge the copper area used. Then in the footprint I could specify that the copper is the same as the pad to avoid DRC errors.
    How do I do this in Allegro? I have a small pad and a large 10.5mm rectangle for this footprint issue above. But I am getting a DRC error from Pad to Shape.
  • steve

    You will always see a DRC in the dra file because this is not net list aware. Once the part is placed in the actual board file the shape will take on the net of the pin so the DRC will automatically be cleared.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.