0
\$\begingroup\$

Clearence between edge of the pour and edge of pad is 9milI am designing a PCB in Altium. I finished my routing and proceeded to Polygon pour for Gnd plane. I was surprised to find the pour in between my 0805 caps pads as well. Although, I don't have a top overlay outline for my caps footprint, but even for components having footprints with top overlay outline, pour is there in between the pins. (I guess, keepout is the one that keeps copper out). I checked Polygon pour options, but couldn't find any thing to avoid it. Is it recommended to have pour in between pads as well? If not, how do it rectify this issue. I have over 60 caps, any shortcuts are also welcome.

\$\endgroup\$
  • \$\begingroup\$ For clarity, please post a picture of the poured polygon and component. I'm concerned that your clearances may be too tight. \$\endgroup\$ – Chris Knudsen Oct 8 '18 at 15:00
  • \$\begingroup\$ Clearance between edge of pour and closest edge of pad is 9mil \$\endgroup\$ – Autobot Oct 8 '18 at 15:12
2
\$\begingroup\$

Polygon pour between component pads is controlled by the standard clearance rule. The polygon is pulled back from pads and tracks of different nets by the distance called out in the clearance rule. You can change this rule (increase the clearance) to control whether or not copper is poured between the pads, but this will also change how much the copper is pulled away from other tracks and pads as well.

There is generally nothing wrong with copper being poured between 0805 footprints, though certain applications may require further consideration.

\$\endgroup\$
  • \$\begingroup\$ I was worried that sometimes parts don't exactly fit on the pads ( either due to wrong footprint dimensions or tolerances), so in that case they have to moved a bit back and forth to solder them. But since, FR4 will be there , there is no risk of shorting the pad with the pour, right? \$\endgroup\$ – Autobot Oct 8 '18 at 14:57
  • 1
    \$\begingroup\$ FR-4 is the fiberglass base material. I think you mean soldermask, in which case yes - the soldermask (like its name suggests) will mask out where you don't want solder flowing. 0805 components are quite large so I wouldn't be at all concerned about shorting between the pads and the pour, provided you have sufficient clearance. Generally I recommend a minimum clearance of 6 mils (~0.15 mm) to ensure your PCB manufacturer can handle it. \$\endgroup\$ – DerStrom8 Oct 8 '18 at 15:50
0
\$\begingroup\$

As @DerStrom8 says, you don't have to eliminate these. But if you really want to, you can use the "Remove Necks When Copper Width Less Than" setting

\$\endgroup\$
  • \$\begingroup\$ Yes. But I tried with clearance setting (between copper and smd pad), which was 10mil before and increased it to 20mils and that worked wonderfully. Although, as @Derstrom8 advised, I let the old setting be. Although, doing this, I found that when settings are changed, present polygon gives error but doesn't readjust itself. Any tips on how to do that? \$\endgroup\$ – Autobot Oct 8 '18 at 16:10
  • 1
    \$\begingroup\$ @Autobot You need to repour the copper by going to Tools -> Polygon Pours -> Repour All. You can also use the shortcut T-G-A \$\endgroup\$ – DerStrom8 Oct 8 '18 at 16:20
  • \$\begingroup\$ Works great.. Grazia \$\endgroup\$ – Autobot Oct 8 '18 at 16:32

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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