PCB Libraries Forum Homepage
Forum Home Forum Home > Libraries > Footprints / Land Patterns
  New Posts New Posts RSS Feed - 0402 Min Size Land Pattern
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

0402 Min Size Land Pattern

 Post Reply Post Reply Page  12>
Author
Message
wolfeman View Drop Down
New User
New User
Avatar

Joined: 19 Mar 2012
Status: Offline
Points: 2
Post Options Post Options   Thanks (0) Thanks(0)   Quote wolfeman Quote  Post ReplyReply Direct Link To This Post Topic: 0402 Min Size Land Pattern
    Posted: 19 Mar 2012 at 11:58am

I have a design with 1mm & .8mm pitch BGAs on it.

Using 0402 caps on back.

Question, does anyone have any input with problems etc using

0402 patterns created using the smallest pattern calculated with current calculator?

If I use smallest pattern 0402 it calculates out to about .56mm sq pads on .84mm centers.

The 1mm BGA works reasonably well with this size 0402 and with gaps in balls on the .8mm part that smallest pattern could work well too.

Any feedback will help.

We really can’t switch to 0201s on this project at this time.

Thanks

Bob

Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5657
Post Options Post Options   Thanks (1) Thanks(1)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 19 Mar 2012 at 1:28pm

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.

Stay connected - follow us! X - LinkedIn
Back to Top
mypal_suresh View Drop Down
New User
New User


Joined: 08 Oct 2014
Status: Offline
Points: 1
Post Options Post Options   Thanks (0) Thanks(0)   Quote mypal_suresh Quote  Post ReplyReply Direct Link To This Post Posted: 09 Oct 2014 at 8:26am

 Hello Tom,
           Can you explain little more detail on 0402 land pattern calculation.

   1.In what all packages we should provide "Terminal " Dimesions as nominal instead of min and max.

     (ex:0201,0402,0603,0805 packages)

   2.Can you be more specific to what is unrealistic tolerances ?

     
     Case 1:    
  
     http://capacitoredge.kemet.com/capedge2/intellispec.jsp?pn=C0402C104K4RACTU&displayPN=C0402C104K4RACTU

        In the above attached datasheet link the terminal dimesion is 0.3 +/- 0.1 mm.

         What would be T min and T max ?

      
    Case 2:

           http://www.mouser.com/ds/2/40/cx7r-218113.pdf

           In this datasheet the terminal size 0.25 +/- 0.15 mm .

           What would be T min and T max ?

Thanks in Advance
 
Regards
Sureshbabu
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5657
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 09 Oct 2014 at 9:19am

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.

Stay connected - follow us! X - LinkedIn
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5657
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 09 Oct 2014 at 9:21am

I highly recommend that you download this new paper on Surface Mount Components -

http://www.pcblibraries.com/forum/surface-mount-component-families_topic1391.html

This paper provides the latest component families and terminal types and their related solder joint goal tables.

Stay connected - follow us! X - LinkedIn
Back to Top
Fynjy View Drop Down
New User
New User


Joined: 06 Feb 2015
Status: Offline
Points: 1
Post Options Post Options   Thanks (0) Thanks(0)   Quote Fynjy Quote  Post ReplyReply Direct Link To This Post Posted: 06 Feb 2015 at 12:21am
Hello Tom.
How will change the designation CAPC1608X90 if I use the density of A, B, C?
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5657
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 06 Feb 2015 at 7:24am
The 1608 is the smallest chip that has 3-Tier Environment Density Levels Least, Nominal and Most).

It depends on which version of Library Expert you are using (Pro or Lite) as to where you change the Environment.

If you are using Library Expert Lite you change the Environment in the "Terminal > Environment" tab.

If you are using Library Expert Pro you change the Environment in "Setup Preferences > User Preferences > Design > Surface Mount Environment > Drop Down" -


Stay connected - follow us! X - LinkedIn
Back to Top
SandroLanot View Drop Down
New User
New User


Joined: 11 Feb 2015
Status: Offline
Points: 13
Post Options Post Options   Thanks (0) Thanks(0)   Quote SandroLanot Quote  Post ReplyReply Direct Link To This Post Posted: 11 Feb 2015 at 2:55pm

Hi,

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

Is there any assembly attachment issues if my 0402 land pattern is 0.40 mm x 0.50 mm, with 1.00 mm pitch?
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5657
Post Options Post Options   Thanks (1) Thanks(1)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 11 Feb 2015 at 3:06pm

Your pad size is the Least Environment. This is good for Nominal.



Stay connected - follow us! X - LinkedIn
Back to Top
jayx View Drop Down
New User
New User


Joined: 29 Mar 2015
Status: Offline
Points: 7
Post Options Post Options   Thanks (0) Thanks(0)   Quote jayx Quote  Post ReplyReply Direct Link To This Post Posted: 29 Mar 2015 at 2:19pm
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.
Back to Top
 Post Reply Post Reply Page  12>

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.094 seconds.