This forum is archived, go to the new forum!

This is the old fritzing discussion forum. Search it for valuable information from 2009 to 2015.

No copper clearance around some or most of SMD Parts

Creekpld 7 years, 4 months ago

if I Copper Fill my PCB Board witch has mostly SMD Parts, there is almost no Cooper Keepout Area around the SMD Parts. I use for Example 0805 and 1206 SMD LEDs, Resisors and Caps. and SOT-23 Transistors All have this problem.

it would also be good, for several reasons to have a separate Cooper and Silkscreen Custom Keepout Area.

Jonathan Cohen 7 years, 4 months ago

Hi Creekpld,

Thanks for the suggestion about keepouts.  

There is actually 6-7 mils of clearance around the smd parts. If you export to gerber and look at the copper layers in a decent viewer you will see the separation. Our production house accepts distances to around 2 mils, so depending on your purpose, the current spacing may be enough. Eventually, as you suggest, we'll make this distance a parameter.


- j


dirk 7 years, 4 months ago

I would like to elaborate and second Creekpld's recommendation or request for a wider copper clearance area / keepout area around SMD parts, when applying a copper fill. Such an wider clearance area would especially be usefull (or even necessary) when doing manually SMD soldering using a soldering iron.

The trick for manually SMD soldering, I'm using -after having secured the component by soldering two corners-, is applying a long strip of solder over all the legs on one side and then removing the excess solder with some copper wick. This won't work if the solder can also creep in other area's, like underneath the component and create shortcuts there. 

The particular aspect of such a special copper clearance area is that it should be formed around the whole part, not just around the individual pins and traces. And notably, that this clearance area is only applicable to a copper fill, i.e. that traces should be allowed in this area (in contrast with normal keepout areas).

It might be just enough to be able to set these clearance areas manually before applying a copper fill - or being able to cut them out of the copper fill after the copper fill is applied.


The photo collage showing the different phases in my pcb manufacturing & assembly might illustrate the particular aspects of such clearance area and the need for it. (See the messy solder on the smd)

SMD Keepout Example


Hope this helps the discussion,




Jonathan Cohen 7 years, 4 months ago

Thanks for that clarification.

In the meantime you could try the trick if you need a way to block copper fill around any area.  I will explain two ways to go about it.

Method 1.  Place three vias on the border of the area you want to protect. You can make them tiny.  Connect each one to the one next to it--in other words draw  a trace from A to B, from B to C and from C to A.  Make the traces as thin as you like.  Add bendpoints to the traces until you have shaped the border to your liking. Now do copper fill--the vias and traces will block it. When you're ready, remove the 3 vias.  

Method 2. Drag out a Logo Image part, and change it from silkscreen layer to one of the copper layers.  Click on the load image file, and load an svg with a simple shape, for example this square:


<?xml version='1.0' encoding='utf-8'?>

<svg xmlns="" width="0.1in"  x="0px" version="1.2" y="0px" height="0.1in" viewBox="0 0 10 10" baseProfile="tiny" >

<rect  width="10" x="0" y="0" fill="#FFFFFF" height="10" stroke="none" stroke-width="0"/>




Now you can copy, paste, and resize this part to mask any regions from the copper fill. Delete them or move them out of the way when you are ready to export.

- j 

dirk 7 years, 4 months ago

Thanks, that's a useful 'hack'! :)