0402 Min Size Land Pattern

Bob,

 

You’re on the right track. Use the “Least” environment for EIA 0402 (1005 metric) chip components. No one should ever use the Most environment for this chip size due to excessive solder.

 

If you normally use the “Most” environment for library construction, use the “Nominal” environment for the 0402 (1005) land pattern.

 

If you normally use the “Nominal” environment for library construction, use the “Least” environment for the 0402 (1005) land pattern.

 

Too much solder on this micro-miniature 2-pin component causes tombstoning in the assembly reflow oven (especially when using lead-free solder).

Here are my recommendations for the largest 0402 (1005) chip capacitor land pattern and it's in the IPC-7351 Nominal environment. I also rounded the corners to reduce the paste mask volume and I would also thin the paste mask stencil to reduce the paste mask volume. However, you can use the "Least" environment dimensions with good results.

 

 

 

One other important rule that you should consider when using Footprint (Land Pattern) calculators for all chip component sizes less than 2 mm (80 mils). When inserting the "Terminal" min/max dimensions, enter the "nominal" terminal dimension in both min/max fields (no tolerance). The component manufacturer's often provide unrealistic tolerances and if you use them for these micro-miniature 2-pin components the resulting pad (land) size is too large.

We had a meeting with IPC-7351 committee last week and we adjusted the "TOE" solder joint goal for parts less than 1.6 mm length. So I have to delete the comment about using only Nominal dimensions for the component terminal because we fixed that in the IPC Calculator in the V2014.11 release.

Here is the new solder joint goal chart for chip components. These new values for miniature parts will eliminate tombstoning issues and provide the best paste volume for the assembly process.

Hello Tom.
How will change the designation CAPC1608X90 if I use the density of A, B, C?

Hi,

This is my 1st post after joining few days ago.

Hello,

I was trying to find recommended land pattern design for the most popular packages like 0603, 0805, SO8 etc. but it turns out to be pretty difficult. I found IPC-7351 and its 3-Tier approach but don’t really understand how can I calculate correct pad sizes using these values. Also I've seen PCB Library Expert SMD Reference Calculator but it returns incorrect values - try to enter 1608 (EIA 0603) package dimensions L=1.6, T=0.35, W=0.3 with ±0.15mm tolerance as found in Kemet datasheet http://www.kemet.com/Lists/ProductCatalog/Attachments/351/KEM_CC103_AUTO_SMD.pdf
and calculated pads will overlap.

Finally I've found information that ModelSource libraries available to download for DesignSpark are created to the IPC-7351 standard. However supposedly also based on IPC-7351 Kemet land pattern design recommendations in document mentioned above (page 12) is slightly different than these in ModelSource. By the way Kemet recommendations are also slightly different for 1005 (EIA 0402) than these in this topic. I know the differences are not big and in real life probably doesn’t matter but would be nice to keep land patterns the same across  the industry. So I'm really surprised there are no exact dimensions specified e.g. in IPC-7351 for the most popular packages.