Print Page | Close Window

Yageo 0603 Resistor Solder Patterns

Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: Footprints / Land Patterns
Forum Description: [General or a CAD specific issues / discussions]
URL: http://www.PCBLibraries.com/forum/forum_posts.asp?TID=2613
Printed Date: 05 Mar 2021 at 5:48am


Topic: Yageo 0603 Resistor Solder Patterns
Posted By: Tom H
Subject: Yageo 0603 Resistor Solder Patterns
Date Posted: 20 Mar 2020 at 12:21pm

The date on the Yageo recommended footprint patterns document http://www.yageo.ru/pdf/R_Mount.pdf" rel="nofollow - http://www.yageo.ru/pdf/R_Mount.pdf is November, 26, 2004. This is before IPC-7351 was released.

The Placement Accuracy noted in the document is +/-0.25 mm. That’s what it was back in 2004. Today in 2020 the placement accuracy of a 0603 resistor is 0.01 mm (10um).

In the 98,000 part Yageo database on POD there are –

  • 1,471 RC0603 series resistors
  • 329 RE0603 series resistors
  • 61 RL0603 series resistors
  • 7,868 RT0603 series resistors
  • 202 RV0603 series resistors
  • 180 SR0603 series resistors

Total = 10,111 0603 Yageo resistors on POD and they all use the IPC-7351 guidelines.

Here is the difference –

IPC-7351 – L pad length = 0.74, W pad width = 0.93 and S pad gap = 0.85

Yageo Resistor 2004 – L pad length = 0.90, W pad width = 0.80 and S pad gap = 0.80

Our conclusion:

  • The Yageo Toe is too big for today’s assembly
    • Potential for tombstoning
  • The IPC Side is too big, but that’s because IPC does not differentiate between chip Resistors, Capacitors and Inductors
    • Resistors do not have metal termination on the sides, but capacitors and inductors do
  • The pad spacing “S” is close (within 0.05 mm)

As a PCB designer, you need to know what Toe, Heel and Side goals are good for your assembly process.

Build your Chip footprint library using a little from IPC and a little from the component manufacturer.

If I was defining the Yageo 0603 Resistor, I would use these values:

PCB Libraries, Inc. – L pad length = 0.75, W pad width = 0.80 and S pad gap = 0.80

I work with a 0.05 mm PCB design and route grid. I want all the features of my footprints to be snapped and rounded to a 0.05 mm grid system.




-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn



Print Page | Close Window