@cjohnson,

Are the pads made as single layer SMD pads with holes placed in the centres and created within the PCB Lib Editor as part of a PCB footprint, i.e. they are not just constructed directly in the PCB editor?

@andyfierman Yes they are created with a bottom layer pad with a hole through the center. If you search for SW-010 in the user contributed library you will find SW-010 and SW-010_BOT. The SW-010 is created with normal through hole pads and SW-010_BOT is created with a bottom layer pad with a hole throught the center.

Um,

Not sure I understand the issue...

I just tried SW-010_BOT in a simple PCB with a top copper area connected to a 9V supply and a bottom area connected to GND. The switch was connected from a 4.5V net to GND:

• I did see some DRC warnings as I redrew the PCB layout (because I was I adding the switch to an existing project) but I made sure to rebuild the copper areas before running the Design Manager and see no DRC Errors.

Copper areas visible:

Copper areas invisible:

• BTW: check with JLCPCB support before you submit the boards that your holes really will not be through or partially through plated when they fab the boards.

I think your second image reviels why you are not getting a DRC error. You manually connected the GND pins of the switch to ground. Remove those traces and rebuild the copper area so that the only thing connecting those pins to ground is the copper area. Typically I dont route GND/3.3V because I'm going to use a plane.

Here's a link to a project that replicates the issue: https://easyeda.com/cjohnson/switch-issue

@cjohnson, @UserSupport,

OK, I see the issue now.

I agree: this looks like a bug.

I am also using non-plated through-hole (NPTH) components i.e. single-layer pads on the opposite layer with a hole in the middle, just like cjonson.

In my case, ratlines continue to show between NPTH pads connected solely by copper areas.

I noticed another bug with NPTH pads in the Photo View:
The holes show as expected on the top layer (1st picture) but the holes don't show in the NPTH pads on the bottom layer. The NPTH pads should have holes in photo view. The plated through-hole pads (terminal block, DC barrel connector and fuse) show correctly.

By the way, my PCB has a number of pads overlapping each other (e.g. large pads for SMT inductors overlapping NPTH pads for through-hole inductors) for flexibility, so it can accommodate different sizes of inductors and current sense resistors. Will this cause any problems with manufacture?

I chose to use NPTH pads because I found plated through-holes to be very difficult to rework i.e. desolder and resolder a new component.

Link to this PCB: https://easyeda.com/tobydante/LV5068_breakout

Top layer:

Bottom layer:

Layout:

Thanks,
Tobias

@tobydante @andyfierman @cjohnson
Hi
Issue confirmed， we will fix it. thanks

@tobydante  @cjohnson
If you want to layout a single layer PCB please refer at this tip:
https://easyeda.com/forum/topic/How-to-layout-a-single-layer-PCB-3f14f6957f0748f18b7dad53bb5d38b2

cc to
@andyfierman

@UserSupport,

Your comment about how to make single sided PCBs is noted but in these examples, @tobydante and  @cjohnson want to make double sided boards but using pads with non-plated-through holes.

@tobydante,

I also noticed that in your Layout image, the outer pair of holes for inductors shows in the bottom (blue) layer but the other 3 pairs do not.

@andyfierman Yes, the inner 3 pairs of inductor holes are 'hidden' underneath the big SMT pad.

Thanks for noting these bugs.

Just to confirm, JLCPCB's Gerber viewer works as expected:

Tobias

Another issue with using single-layer pads with holes in them for through-hole components is that these pads are included in the paste layer, which I think is meant for surface-mount components. In the Gerber image below, the plated through-hole pads are not on the paste layer, as expected, but the pads with non-plated holes are on the paste layer, which they shouldn't be.

I want to make a stencil for PCBs like this one. At JLCPCB, is the stencil cut according to just the paste layers? If that's right, my workaround is to order the stencil with the Gerber of the PCB design with only the surface-mount components. As a stencil's design area is 190x290 mm, I am thinking of combining the SMT pad patterns for multiple PCBs on one stencil.

It would be preferable if a pad can be set to a single layer but still have a hole in it, set by its 'Hole(D)' property, rather than having a separate hole placed over the pad. This way, such pads can be excluded from the paste layer.

Thanks,
Tobias

@tobydante We will see what happens. I ordered the boards from the original post as is, we will see how they show up!

I experimented around with doing a cutout on the Paste Mask Layer.

This does not work. The gerber still shows up with cutouts for the stencil.

EasyEDA probably assumes that if the pads are originally created as SMD pads (which they are if they're on only one top or bottom layer) then they should have solder paste on them.

@andyfierman One particular case where that definitely wont be true is the TC-2030/50 connectors. They are footprint only programming connections. Here's a link to them: http://www.tag-connect.com/what-is-tag-connect

Datasheet for the TC2030: http://www.tag-connect.com/Materials/TC2030-IDC.pdf

It isn't recommended to deposit solder paste on to these pads.

Other examples would be plated fingers for edge connectors, test pads for pogo pins (similar idea to the Tag Connect parts) and things like pads for connections to wire-in-silicone emc gaskets.

A question for EasyEDA and JLCPCB support?

@andyfierman Good point.

Are we looking in to adding in the feature for this?

Why doesn't a "cutout" on the Paste Mask Layer disable paste in those areas in the gerber files?

@cjohnson,

My specialty is in design and simulation so that's a question for the developers.

This thread has made me realise that there is quite a lot I don't know about how EasyEDA handles some the PCB features.

@andyfierman
Well one thing I would add to this, is just how significant EasyEDA is. The company I work for has used Ultiboard/MultiSim, PADs and some other flavors of software. EasyEDA is miles ahead in terms of ease of use, creation of libraries, visually easy on the eyes, features, support and cost (well duh).

I've personally moved us completely over to EasyEDA, as it is so much easier to manage/create libraries and boards. What used to take me a few days in PADs or Ultiboard I can now do in a day and have the board ordered.