Pad to track clearance missing?

Layout
1

Edit: Paulvdh

This “same problem” refers to the thread this was split off from:
Way to set copper pad clearance different than track clearance? - #16 by SembazuruCDE

I have the same problem. My fab can do 250um track clearance and I want to have a single sided board without a mask due to cost reasons (my first PCB for personal project). But, I cannot hand solder a pad with a bare copper track just 250um next to it without making a solder bridge. In other words, I want tracks to be have 250um clearance, but pads to have like 1mm clearance for easy hand soldering. This still cannot be set globally. What I can set is hole to track clearance which works for holes only and I will have some SMD resistors on the board as well.

See the picture. I want to set a “pad to track clearance” rule which would apply to both highlighted problems. Such a rule doesn’t exist globally, only locally for every pad (as a clearance). Setting the clearance on one pad and “pushing the pad properties” to other pads does work for similar pads of similar components, but I need to set this for all therefore I need a global setting.

Or maybe I missed a setting for clearance of SMD pads?

image
image826×636 39.3 KB

2

Or maybe I missed a setting for clearance of SMD pads?

You didn’t miss a setting. But you missed the opprotunity to use the custom rules. With these custom rules you are able to implement specific DRC-checks according to your needs.
Please read the corresponding section in the documentation: PCB Editor | 6.0 | English | Documentation | KiCad

short steps to get you started:

  • in board-editor: File–>board setup
  • section design rules → custom rules
  • first click on “syntax help” (top right corner), the help-window shows a short description and some more commonly used rules (look at “more examples” → there is already a “pad to track”-rule) These examples can easily be copied into the rules-window.
  • if you directly want something to copy: paste the following 4 lines into the “custom rules”-dialog window:
(version 1)
(rule "Pad to Track Clearance"
    (constraint clearance (min 1.0mm))
    (condition "A.Type =='Pad' && B.Type =='Track'"))

(Edited by eelik: " " are changed to other characters and don’t work when copypasted if they are not inside a “preformatted text” section.)

1 Like
3

I guess my needs aren’t frequent enough to justify having an option for it. Custom rules with a specific syntax is a generic solution and I understand those are more desirable to have in a software (am a software developer myself). I will use this custom rule then. I was afraid these rules would only be checked when DRC is run specifically, but actually it’s respected when routing tracks live so that’s good.

Thank you.

4

Well, this is good for routing but I cannot see the custom clearance when placing components manually so it’s still not great. When I set the clearance on every pad, the clearance is visible when placing the component.

I will redefine what I need more clearly. I need this (the pad clearance field) but set globally. Or maybe an easy way to set this on all pads.

image
image1046×682 31.7 KB

5

Or maybe something like “change pads on all footprints” in this window? That would be a generic solution.

image

6

I will redefine what I need more clearly. I need this (the pad clearance field) but set globally. Or maybe an easy way to set this on all pads.

I learned some days ago that this is called xy-problem.
You have already expressed your problem (more clearance on pads, less clearance on tracks). Try again (more creatively) with the custom rules.

hint:

  • set normal netclasses to 1.0mm (==clearance for all elements on whole board) → this enables your desired “clearance-circles” around the pads
  • and than use a custom rule to get smaller clearance for track-track :
(version 1)
(rule "Pad to Track Clearance"
    (constraint clearance (min 0.2mm))
    (condition "A.Type =='Track' && B.Type =='Track'"))

If you still insist to use the pad-clearance-setting:

  • upgrade to v7 (current release candidate, called “nightly” on the kicad download page)
  • enable properties-panel
  • selection-filter: enable only pads
  • CTRL+A selects all pads from footprints on the board
  • use the properties-panel to set Clearance Override == 4.0mm

I strongly disadvise this (my own) suggestion:

  • every footprint-update from library will delete your changes
  • all clearance-changes from the netclasses have suddenly no effect on pads (as opposed to most other boards)
  • both points will create problems in the future - at the time when you have forgotten your trick done to the board (if this is a one-off board both arguments are not applicable)
1 Like
7

Probably. Standard two sided boards with solder mask are usually extremely cheaply mass produced and will usually be easier to manufacture.

If you’re doing special stuff, like milling the boards yourself, you might also need to do special stuff in KiCad.

8

Oh yeah, defining global clearance and then changing track-to-track clearance is a good idea. Haven’t tried it thought.

It is my first board and it’s a one-off so I don’t mind the tricks with this one. I will likely design more boards in the future and I will try to do things the proper way as I learn.

Thanks to everyone involved. I am glad to see KiCad has an active community of experienced users.

9

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.