Simple via and mounting holes troubleshoot

[spiros]

Hello there,

I’ m on my way on finishing my simple PCB design. I try to add a hole through which i will connect the top and bottom filled zones, which in my design is the ground. The idea for this is to be a simple hole, not filled with copper (for lower manufacturing cost), where i will place a pin and solder it both on top and on bottom, so the filler areas (ground) will be connected to each other.

I added a via hole, hoping that this will do the job. By doing this, first of all, on pcbnew i get what looks as a a drilled hole, surrounded by a large white circle which as far as i understand stands for via. My values are “via: 3mm, drill hole 1mm”. This white circle looks quite similar to the lines indicating outlines because of the colour. Is it meant to be a line indication or as some kind of inductor material that connects the two layers?

After that i placed some single pin pads in order to manipulate them as mounting holes for the PCB. Their drill size is 3.2mm and the pad size 5mm. Because i didn’t figure out what the outcome of the via would be, i though of also using this single pad, placed at the exact position on both PCB layers, in order to use it as a connection gate, instead of my via hole. But when i go to 3D view i see that both the via and the mounting holes do not have a hole drilled, while all of the drill holes for the components are empty.

At the edit tabs of all of the holes i have similar settings. Could i be missing something? Or could it be that the 3D viewer is not getting all the info, and that on the actual result they re gonna be drilled?

Furthermore, as i see the mounting holes, they 're gonna act also as a connection point for the PCB ground to the chassis, since the PCB is gonna be mounted directly on it. I guess if i didn’t want this connection to happen, i would need to remove the filled areas and then refill it, so the holes would have an isolating area around them, right?

thanks in advance for any help,

Spiros

[Joan_Sparky]

@spiros

The idea for this is to be a simple hole, not filled with copper (for lower manufacturing cost), where i will place a pin and solder it both on top and on bottom, so the filler areas (ground) will be connected to each other.

You wont save a dime…
Normally a joe-average PCB starts with a prepreg that has a very thin copper cladding on both sides, that is modified to resemble all your traces/zones/etc via etching (fast & cheap to etch away a thin copper layer).
This then is put into a bath that contains solved copper which will chemically bind to the cladding and increase it’s thickness to usually 0.35u. At the very same time any other ‘unprotected’ surfaces (including holes) will also be plated with copper.
There is no additional cost.

Please use 30 min of your time and watch this video:

Eurocircuits - how to make a 4-layer PCB (full version)

The difference between PTH (plated through hole) and NPTH (non plated through holes) is when they are created along the steps of manufacturing your pcb.
PTHs are made (drilled) very early (same time as vias) to get their plating.
NPTHs are made before the milling (or with it, depending on process), as they they don’t get plated.
Usually the manufacturer will adjust the drill size for the drill holes in the PTHs, so that the final plated hole size is what you specified…

PS: that is also why most fabs/aggregators need PTH/NPTH specified in separate drill files, while some do depict that information from copper being ‘over’ the hole for plated holes.

PPS: for your reference…
z_MountPTH_3.0mm.kicad_mod (688 Bytes)
z_MountNPTH_3.0mm.kicad_mod (690 Bytes)

[spiros]

Thanks a lot for your help Joan,

It is really important for a designer to understand the method that will be used for the manufacture of the design of his or hers. I understood a lot of the steps taken in the manufacturing process of a PCB by watching the video you suggested. I am not sure yet about where i will actually send my design to be manufactured though. Most big facilities would use similar procedures, but smaller facilities may not? I m thinking about it, because one local manufacturer that i contacted (location : Greece) asked me for pdf files in order to print transparent sheets and proceed to the manufacture… I would like to try their product, because if the quality is good, i will be able to have the boards made in a short period of time. Judging by their pdf requirement, I think they wouldn’t be using the prepreg and baths technique…

But, leaving that aside, what would be the colour translation of the via hole i made at my design? The white outer circle indicates connection between the two layers and the black hole a drilled hole? And why i am not able to see any drilled holes at the mounting and via holes on the 3D view mode? Another weird thing is that now that i reopen my layout on pcbnew, the via hole doesn’t actually look like a hole any more. It looks “copperous”. Mysteries of life! Also holding the cursor over it and pressing E does not open the edit tab.

@Joan_Sparky

PPS: for your reference…z_MountPTH_3.0mm.kicad_mod (688 Bytes)z_MountNPTH_3.0mm.kicad_mod (690 Bytes)

I also added your pads to my board and at the 3D view i still do not see any holes…

It seems to me, that either i miss some simple things, or something is going wrong…

[bobc]

@spiros

asked me for pdf files in order to print transparent sheets and proceed to the manufacture…

Really?? I’ve never heard of any commercial outfit using PDFs, hobbyists maybe. If you are starting out it is probably not a good idea to choose an outfit with weird production techniques, even if they are incredibly cheap and you are on a budget. If you wait a little, there are many fab houses which are cheap, have good quality and ship globally.

Pcbnew display vias as white circles. If you turn off “Through Via” in the Layer manager then if they are vias the white circles will disappear.

In the 3D view, it looks odd. I’m not sure older versions displayed holes correctly. You have an odd color scheme, but I am wondering if the solder mask or some other layer is covering the holes.

FWIW, my boards appear like this in 3d viewer:

What version of KiCad are you using?

[Joan_Sparky]

@spiros

I also added your pads to my board and at the 3D view i still do not see any holes…
…
It seems to me, that either i miss some simple things, or something is going wrong…

I just addded them to a test board and they look like this:

These are the settings for the 3D viewer:

[spiros]

Thank you for your replies,

some things look clear already.

@bobc

Really?? I’ve never heard of any commercial outfit using PDFs, hobbyists maybe. If you are starting out it is probably not a good idea to choose an outfit with weird production techniques, even if they are incredibly cheap and you are on a budget. If you wait a little, there are many fab houses which are cheap, have good quality and ship globally.

Yeah, pdf sounds weird, after giving all that effort to create the gerber file… I ve already even found some platforms to choose from different manufacturers globally. I just though to give it a try with the neighbour. More immediacy. Since it is a standard technique to have the holes coated though, it would be bad to lose it…

@bobc

Pcbnew display vias as white circles. If you turn off “Through Via” in the Layer manager then if they are vias the white circles will disappear.

This worked out.

The colour scheme of the 3D viewer is the default. Some information about the version i use, installed in my ubuntu studio system:

Application: kicad
Version: 4.0.6-e0-6349~53~ubuntu16.04.1 release build
wxWidgets: Version 3.0.2 (debug,wchar_t,compiler with C++ ABI 1009,GCC 5.4.0,wx containers,compatible with 2.8)
Platform: Linux 4.8.0-46-lowlatency x86_64, 64 bit, Little endian, wxGTK
Boost version: 1.58.0
Curl version: libcurl/7.47.0 OpenSSL/1.0.2g zlib/1.2.8 libidn/1.32 librtmp/2.3
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_WXPYTHON=ON
USE_FP_LIB_TABLE=HARD_CODED_ON
BUILD_GITHUB_PLUGIN=ON

I cannot understand the colour scheme of your 3D viewer, since i am not familiar with different kicad editions… If the light green colour is meant to represent the background of the 3D viewer then the holes are visible…

But as Joan very correctly suggested, i clicked on: Preferences --> Render Options --> Show Holes In Zones, and after that i can see the holes in 3D view

I don’t see anything special on via’s 3D representation though, that would indicate that this passage will act as a via, connecting my bottom to top layer. Is it supposed to indicate it somehow or i 'll just have to trust the system?

Would anyone have some advice on the proper way to create PCB mounting holes? I would make them NPTH and i would also need no copper present at a circular perimeter around the hole, so when i tighten the metallic screw it would just lay pressed against some non conductive plastic.

thanks for all the help,

Spiros

[Joan_Sparky]

@spiros

Would anyone have some advice on the proper way to create PCB mounting holes? I would make them NPTH and i would also need no copper present at a circular perimeter around the hole

I would have expected NPTH & None in the copper layer settings would do the trick, but some internal KiCAD logic does prevent that.

So to do it, you have to use 2 elements placed over each other instead of just one:

• NPTH hole
• SMD pad (diamater how you want) with copper set to None and F.Mask/B.Mask ticked

[Sprig]

NPTH Mounting Holes ... AAAaarrgh! Or, how to get them right the first time

Well, I THINK have them figured out now, but it has taken me several hours for 2 friggen holes… LOL To have a great search-able post, I’ll work through the steps here. Make any corrections or suggestions and I’ll edit this OP. 1) Help me Obi-Wan Kenobi, you’re my only hope… Open PcbNew, and depress the “o” key (( or left click the “Add Component” button) (or find it in the menu bar)), then click the location on the board where you want a mounting hole. A new window will pop-up, and I recommend…

It was not easy for me either… Hope This Helps.

[spiros]

@Joan_Sparky

So to do it, you have to use 2 elements placed over each other instead of just one:

NPTH hole
SMD pad (diamater how you want) with copper set to None and F.Mask/B.Mask ticked

Hole h1 is made like you suggested. What i find different from yours as a result, is that mine has two different colours at 3d view. One for the inside of the hole, that when comparing to the other holes next to it i can understand that the colour coding means that no copper is in the hole (NPTH). But the red circle, which is the smd, no copper pad is represented in red. On the three pin pad, right above h1, i see this red circle perimeter laying on the pads where i am gonna place a component. at the bottom side, i get the exact same behaviour, just in different colour (green). Wouldn’t these circles represent some copper traces where you would actually solder your components? I am not familiar with the colour coding of your 3D viewer, but at least you have the same colour in the hole and on the board’s surface. So if the hole is empty of copper, i would imagine the board being too.

Afterwards, by reading Sprig’s post, i noticed down some facts, as that there is a library with mounting holes, where there are already available various options. h2 is an NPTH 3,2mm circular hole and h3 a through hole (PTH) 3,2 circular hole. I have difficulties in understanding what the outcome is gonna be of the physical PCB, by translating this color coding.

Here you can see the board on pcbnew

and here i found a maybe nicer 3D preview mode called realistic mode

So, do you think that the h1 hole is gonna be with no copper on it’s perimeter after all?

[Joan_Sparky]

I found the realistic view always better than the one, were the colors try to replicate the scheme from the 2D editor.

What I can see in the realistic view:

• h1: large non-soldermask area, NPTH
• h2: plain NPTH with with some soldermask setback (probably from global setting)
• h3: PTH with soldermask setback, probably due to PTH settings

None of them look like what you wanted as in all cases the copper fill zone doesn’t stop some distance before the hole.

And after some more trying I found what you have to do.
Use a plain NPTH and adjust the net pad clearance for that footprint locally like this:

[spiros]

Thank you for your effort Joan, i appreciate that,

I followed the steps as you described them, but i still can’t get a satisfying result in 3D view.
Here i present an example of four new holes a i made.

All of them have the same setting on Pad Properties “General” tab.

h4 has everything set to zero at “Local Clearance and Settings” tab

h5 has net pad clearance at 15 mm as you suggested.

For h6 i set Solder mask clearance to -5

And for h7 i tried -5 for Net Pad clearance and -5 for solder paste clearance

I would except to have a circle with the same colour as the inside perimeter of an NPTH for a non copper result.

I read some documentation about pad properties. On chapter “13.8. Adding and editing pads”, i read there the intention to be able to create clearance for screws, but there is not a specific guidance:

Non-plated through hole pads

Pads can be defined as Non-Plated Through Hole pads (NPTH pads).

These pads must be defined on one or all copper layers (obviously, the hole exists on all copper layers).

This requirement allows you to define specific clearance parameters ( for instance clearance for a screw).

When the pad hole size is the same as the pad size, for a round or oval pad, this pad is NOT plotted on copper layers in GERBER files.

These pads are used for mechanical purposes, therefore no pad name or net name is allowed. A connection to a net is not possible.

I m starting thinking of the idea of using some kind of rubber bushing in the end, like this one

Although I would prefer to learn a more proper way of designing…

[Joan_Sparky]

Did you hit [B] (refill zones) after placing those footprints or changing any settings on them?

The settings preview for h5 look to me, that KiCAD knows what to do.

Be aware that the clearance is a radius from the edge of the copper outer radius (or outline) - for NPTH this coincides with the drill radius.
So in your case the outer diameter of that h5 footprint becomes 15+3.2+15 = 33.2mm

Also for h6 you tried a negative soldermask clearance, which would be towards the copper and not away from it.

Try this:

[spiros]

Oops… That was it.!
Refill zones let me fulfil the task!

Setting Net pad clearance 2 and solder mask clearance 16 gave me a weird looking result with a huge yellow surrounding area.

but lowering solder mask clearance to 2 got me there

Also lowering solder mask clearance even more amd making it 0 while keeping net pad clearance to 2 gave me an interesting result. As i can tell from the image of the trace, at the top right corner of the image below, the dark green area, shouldn’t be conductive. I am not sure about the differences of the brown and dark green areas of the PCB, but i think that this orientation would also work.

What appears as a problem, after refilling areas in all the zones, by pressing B, is how the via connection now appears. It became an island, with no connection to the land around it. I tried pressing E for edit or right clicking to try to edit it’s preferences, so i could connected to my desired net, but i wasn’t able to find the way for it. Pressing E on it erases a circle on it’s PCBnew graphical interface, and by right clicking on it, i only get an option for editing all tracks and vias, where i cannot select a net.

Afterwards, by looking also in other posts, i tried creating a track on a pad of the desired net i want to connect and after a while pressing V to make it a via and then double clicking to set it.

On 3D mode i see just a hole. no connection. (this hole would maybe do the job though, as it looks like connecting the two sides…)

If i press B after the set of the via i get this

still the two sides do not look connected

and backside

I guess i should somehow set the net connection of the via while creating it, but i cannot seem to be able to locate how to do this…

[Joan_Sparky]

[quote=“spiros, post:13, topic:6025”]
What appears as a problem, after refilling areas in all the zones, by pressing B, is how the via connection now appears. It became an island, with no connection to the land around it. I tried pressing E for edit or right clicking to try to edit it’s preferences, so i could connected to my desired net, but i wasn’t able to find the way for it. Pressing E on it erases a circle on it’s PCBnew graphical interface, and by right clicking on it, i only get an option for editing all tracks and vias, where i cannot select a net.[/quote]

A via in KiCAD always needs to be connected to a track, otherwise it will lose it’s net and become free floating and be disconnected from the net it was connected to before… (see ‘via stitching’ as a search term on this forum for discussions on this very subject).

@spiros

Afterwards, by looking also in other posts, i tried creating a track on a pad of the desired net i want to connect and after a while pressing V to make it a via and then double clicking to set it.

That’s how vias are being created, correct.

@spiros

still the two sides do not look connected

Look up the properties of each filled zone.
Check the net setting on each.
The via/track will only connect to either zone, if they have the same net…

[spiros]

@Joan_Sparky

Look up the properties of each filled zone.Check the net setting on each.The via/track will only connect to either zone, if they have the same net…

My zones were both created as Net-(C1-Pad2) so they should get connected. Checking at the Edit Zone Properties tab that you suggested i found them being set to this exact Net. After trying a couple of times clicking on them and exiting this tab by clicking ok i somehow managed to get it working. Now by pressing B i don’t get the islands.

I didn’t quite understand what was the change that i achieved. It seems that for some reason now, the program has accepted both zones as being the same net…

But i think that finally i established a correct via connection. What do you think?

[Joan_Sparky]

@spiros

But i think that finally i established a correct via connection. What do you think?

Looks alright, final check is the gerbers though - as those communicate your specs and intentions to the guys making your board