I'm trying to add a DRV8301 componenet (Texas Instruments) in Eagle and it's my first time. So the componenet package is DCA as indicated in the datasheet.... i followed the dimensions to make this one. and this are images with the dimensions in mm of the componenet that i maked[!

enter image description here

i've chosed a grid size of 1mm

so i want to know if my componenet is adequat to the datasheet .... thank you

  • \$\begingroup\$ It looks "close" but there are a few issues. "close" can mean the difference between it working or not. For one the datasheet asks for a Non-solder mask defined pad, so you will actually need to pull back the solder resist from the what eagle typically does by default. It appears that you set the inner pad dimensions to match the stencil opening, not the recommended land size. \$\endgroup\$ – crasic Oct 16 '15 at 19:43
  • \$\begingroup\$ My typical strategy is to make a single pad with the correct dimensions, solder resist,etc., then use a spreadsheet and the datasheet to calculate the origin positions of every pad, then copy and move, by setting Position to the calculated points exactly. Once you get the hang of it, this can be automated using an eagle script generated directly from your spreadsheet \$\endgroup\$ – crasic Oct 16 '15 at 19:44
  • \$\begingroup\$ well i'm still new using eagle ...so i didn't quite understand what you said .... i've looked every where for the component library or the package TSSOP 56 but i did not find anything :( \$\endgroup\$ – Anoir Nechi Oct 17 '15 at 16:22

There are 2 seperate questions here

  1. Is this footprint matching the manufacturer recomendation

  2. Will this footprint work with my design and board manufacturer

There are subtle differences but they can matter.

For #1 I believe you have neglected a few relevant details that may impact the performance of the part.

The Datasheet specifies the recommended shape and form of both the copper pad as well as the solderesist layer above. The relevant diagram is reproduced below

enter image description here

The relevant layer for defining the solder resist in eagle is either tStop or bStop depending on the side of the baord. The datasheet is suggesting a copper pad 14mm by 5mm with an exposed center (tStop box) 6.35mm x 3.61mm in the center which roughly matches the size of the exposed thermal pad.

There are a few reasons for and against using this type of soldermask defined pad and you do not have to follow the recommendations exactly. However, the extra heat sink of the pad may be necessary for reliability. But, making the finish flat requires a little more care from the manufacturer.Depending on your design or chosen manufacturer the concerns shift hence the difference between question #1 and #2. Confirm with the manufacturer that any thermal vias you place under the solderesist won't raise the IC (requires a different plating process).

For the pins, they recommend a Non soldermask defined pad which is covered in other questions like Eagle - non solder mask defined (NSMD) pads and solder-mask-and-cream-in-eagle. The manufacturer recommends using this pad type. Eagle by default leaves a solder resist gap.

I am not sure what dimensions you took for the pins, but it should be a little longer and wider than the physical pin, the recommended dimensions in the figure are 0.3mm x 1.5mm

| improve this answer | |

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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