Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
Yes you can, these components are used on very dense boards I have used the IPC-7351 least footprint and had the placement outlines touching and had no problems with assembly or re-work.
Yes you can do this, But if the component assembly or rework is in hand soldering means doing repeatedly will be an issue. Whereas if it is machine assembly it should give you no problems.
The only issue that I see is if these components are resistors dissipating near to its rated limits, due to reduction of the effective area designated to heat flowing from each one.
I agree with all above posts. My only warning is - if you are assembling the boards using a standard stencil, you may want to deviate from the standard 5-mil steel and reduce to a 4-mil or 3-mil. Even if paste is applied to each pad properly, the surface tension during reflow will cause a bit of movement. The risk is that you will end up with a solder bridge, which is the worst to fix on 0201's due to their size.
Also note that many assembly companies want some amount of space between components - not between the pads but between the outside of components, as pick and place machines all place within tolerance. You don't want to have one resistor placed a degree or two off and have it bumped off the pads, causing a ton of rework later.
In most cases, assembly houses will assemble PCB's using IPC-A-610 as a standard for quality control. In IPC-A-610, three classes are defined;
Class 1
Class 2
Class 3
This standard does not define the distance between to components but defines the allowable overhang of a component.
This allowable overhang determines the minimum distance between the two components. If you are planning series production of the design
you should take these values into account.
I would kick my assembler from here to Kathmandu if any components were that far off the pads, though I must admit out of millions of the little buggers placed over the years I have only seen them that bad twice....
The problem is with todays tight designs and copper flooded everywhere there is a chance of shorts, which is what happened in one of the cases where the comp was off the pad...........
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.