I'm creating footprints for some components. For SMD resistors and capacitors (R0603, C0402, etc.) there is a recommended land pattern in the datasheet of each component. For example, a Vishay R0603 resistor has a recommended land pattern which is slightly different from that of a Yageo R0603 resistor.

Is it advisable to create a specific footprint for each component brand, for example a Vishay-R0603 footprint, a Yageo-R0603 footprint and so on for all manufacturers or can I use a generic R0603 footprint and be pretty sure not to have problems during assembly for all resistors with 0603 package of any brand?

If so, is there an "official" document that lists the standard land patterns for the various SMD packages?

  • 1
    \$\begingroup\$ It might help if you showed the two slightly different footprints and explained where the slight differences occur. \$\endgroup\$
    – Andy aka
    Jan 23, 2023 at 12:56
  • \$\begingroup\$ I have never bothered. Even for things like those flat MOSFETS in 2.0x2.0 mm or 3.3x3.3 mm packages, using the same footprint for various manufacturer parts has been no issue. I guess those super detailed recommendations in datasheets have the main purpose of reassuring customers that that particular manufacturer is very mindful of details, and not necessary for actual manufacturing, which would probably depend much more on paste type and temp profile (i.e. solder expertise). \$\endgroup\$
    – tobalt
    Jan 23, 2023 at 13:00
  • 1
    \$\begingroup\$ If you use a different land pattern it can have an effect on the device depending what it is etc. It may also cause warranty problems. The manufacturer gives the foot print for a reason. My recommendation would us what the manufacturer specifies. \$\endgroup\$
    – Gil
    Jan 23, 2023 at 13:58

2 Answers 2


If we are talking about mass production, the best course would be to ask your assembler for a land pattern (at least for 0603 and smaller). They know their processes best an can recommend land patterns that worked perfectly fine a million times.

The recommended land pattern from every reputable manufacturer should be a good choice, too. But I wouldn't worry too much about the small differences between them. Maybe just use the "mean" land pattern.

Then there are IPC standards for land pattern design and solder joint goals (IPC-7351 and J-STD-001), where you can calculate land patterns based on the part's dimensions (there are also third party tools that can assist you with that). But for chip components like 0603 and smaller I would use IPC only, if there is neither a good manufacturer nor an assembler recommendation.

In a nutshell where to get your land patterns for 0603 and smaller from with 1. being the highest priority:

  1. Assembler's recommendation (if applicable)
  2. Manufacturer's recommendation
  3. IPC guidelines/standards

Yes, there are indeed standards for this.

Please have a look at IPC footprints. You will have to buy the full document.

A quick Google search can provide useable results - based on IPC - for common packages.

If you are planing to do high-volume production, my advice is: Talk to your assembly house. They know their processes and tweaks. They will provide footprint/paste recommendations based on real-world applications for almost any package and application.

The reason for this is: Today you are using the Vishay type resistor, tomorrow the same 10 kΩ 5% 0603 is 5 cents cheaper from a different brand, so you use this one for non-critical components. Therefore, using manufacturer specific footprints "locks you in." Furthermore, your assembly house may have specific knowledge regarding their process - giving a 2mil wider pad may result in 1% more yield in their process. Let them do their magic.

If you are doing mid/small-scale production, use the IPC standards; they won't be perfect, but good enough to get high-enough yield.

The reason is that most likely you will do batch production, therefore you can never know which type of resistor is available. Of course you can buy a 10k piece reel and store it between batches, but this is expensive so you want to use a generic approach. Furthermore, you may even switch assembly houses between batches. Using the "industry default" IPC-landpatterns will not be optimal but will fit all assemblers and requirements.

If you are doing hobby-scale products, just don't care. Use one common footprint and you are good to go - your CAD package will have these available already.

Regarding warranty:

If you use standard packages (be it passive or ICs) there will be no warranty problems by using a generic IPC footprint - and your asembly house (if creditable) will know about long-term issues in their footprints.

If you are uing some "fancy-pants" package, then I would go with the manufacturer advice and talk with my assembly-house to see if they can see issues regarding yield.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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