Where to set global pad clearance?

Layout
1

I must go crazy (or blind), but in the current RC1 version of KiCad I’m not able to figure out where to set the global solder mask and paste clearances for pads.

Any hints?

2

Never mind, found it in the Layout Editor > Dimensions > Pad Mask Clearing.

However, the OpenGL footpring editor insists in rendering a largish solder mask clearance, even when everything, including the global clearance, is set to 0. Bug?

3

Did you check the pad clearance of the footprint and then of each pad?

footprint:
Footprint editor > Dimensions > Pad Setting > Local Clearance and Setting

pad:
select pad and click [E] > Local Clearance and Setting

If both are set to ‘0’ then you got a bug, otherwise your footprint or local pad settings are in charge

4

@chicken - It is a bug. Fixed in 4.0.5. Kicad->PCB Editor->Dimentions->Pads Mask Clearanse - set Solder mask clearance to 0 (or to 0.02mm)

5

Version: (5.1.5)-2, release build

Who stole the menu?

OK, so where do you set global pad clearance nowadays please?

Four years ago “Chicken” asked the same question. I’m hoping I’m not going to be embarrassed by an RTFM message because I’m really happy to read any amount of documentation if someone can simply point me at the latest relevant stuff. I looked in all the docs that popped up when I googled “gloval pad clearance”, so I guess I must be word-blind or something? There are plenty of references to a mysterious “setup” menu, but I don’t have one of those on my menu bar.

.

6

The global solder mask clearance dialog in Pcbnew (the board editor) is under File -> Board Setup -> Solder Mask/Paste:

image
image1376×872 52.4 KB

2 Likes
7

Solved. The issue was more complex than I appreciated - I think because the somewhat non-bvious UI has rushed ahead of the documentation. Previous descriptions referred to a main-menu item that has now been pushed into the PCBNew “board setup” dialog. In digging around I learned four new and useful things that other noobs might not learn in the normal course of things.

  1. Pad clearance is derived from the net class of the connecting wire - usually the default net class. There are probably other inheritance paths for path clearance I don’t yet grok.

  2. Make sure that you set up the minimum track width in PCBNew: Board Setup/Design Rules to be less-or-equal to the track width you need to get into the target pad. Click on the actual text “Design Rules” is you wonder where this control panel is lurking. If you don’t do this the UI will squeak when you try to define a path (below) smaller than your minimum.

  3. Set up a new net class with an appropriate track/via width etc. PCBNew: Board Setup/Design Rules/Netclasses Assign your new netclass to the appropriate wires. This is done by selecting a wire by-name, and assigning a netclass to it! The interface provides a mechanism to filter down the complete netlist to a subset of names containing a specified string - for example “U2”. The desired new netclass name can be assigned to all of the results of the filter, or just the ones you select.

  4. When routing it helps to set the router settings to Highlight Collisions. Then you see the issues instead of the more perplexing behavior where mouse clicks appear to have no effect (to this Bear of Little Brain anyway) PCBNew: Route/Interactive Router Settings/Highlight Collisions.

Once I had that all set up I was able to route to the tiny pads that resisted my attentions earlier.

1 Like