Footprint for bracket, hole not showing in 3D view

[Douglas777]

I am trying to do a footprint for a simple mounting bracket:

This will be used to mount a PCB to a panel.
For the face of the bracket to which the PCB is attached, I am thinking that the footprint should be a pad which is the size of the bracket face,
together with a PTH.
The symbol has a corresponding single pin 1 for “chassis ground” (elsewhere in the schematic I can connect that to the system “star ground”).

My approach for the footprint was to use a rectangular “surface mount” pad (“pin 1”) for the front copper and ditto for the back copper (without any pin number).
The hole for the mounting bolt is a pad of type “Through-hole” (without a number), which I understand provides a PTH (which will link the FC and BC pads).

Is my approach reasonably sound?
However, for the 3D view the hole is not seen.
The hole does show when the 3D view is rotated to look from the back face of the PCB.
So the question is “why does the hole not showing in 3D view”?

I also attach the footprint file
Keystone617BracketMainPCB.kicad_mod (2.4 KB)

[paulvdh]

The grey stuff is solder.

Turtn of the (solder) Paste layer for the SMT pad.

[Douglas777]

Thanks for this explanation!

Assuming I wanted to get a stencil from, for example, JLCPCB, would I need to have the F.Paste box ticked?

Or, is it sufficient to have the F.Mask ticked?
As I understand, mask acts in the negative sense - where mask is drawn, it defines the area free of soldermask - which implies where paste would be used.
Do JLCPCB, etc., base their stencil production on F.Mask and/ or on F.Paste?

For the purpose of obtaining a stencil, I would need to have both F.Mask and F.Paste ticked for every footprint?

I see that it is possible to turn off the solder mask layers in the 3D viewer which resolves the issue of being able to see the holes whilst also being able to have the footprint ready for its usage.

[paulvdh]

F.Mask is for the solder mask, which is the (usually green) paint on your PCB.
F.Paste is for the solder paste, which is the tacky grey stuff with solder balls and flux and these end up as the holes in the stencil.

This seems fairly logical and straightforward to me, so I wonder why you are confused.

This bracket looks like it’s going to be screwed to the PCB. If you want it to be an electrical connection, then you probably do not want solder paste on it. Solder creeps under pressure, and this diminishes the clamping force over time.

If you want something complicated, you can use an “aperture pad”. and SMT Aperture pad has it’s copper layer disabled, and also does not have a pad number. This is used if you want layers such as the solder mask or paste to have a different from then the copper. (In this case you disable those layers on the “real” pad.

[eelik]

The mask layer and the paste layer are two completely different things. The mask layer is negative, yes (How does solder mask layer work?), but it’s the paste layer which is solely responsible for the paste stencil.

That said, it would be an error to have paste where there is no soldermask opening and no bare copper, because it’s meaningless and detrimental to try apply paste to where it can’t be attached. The manufacture may or may not ask you if you try to order a stencil which they see isn’t fitting for your board. But again, it’s made according to the paste layer, not mask layer.

[mf_ibfeew]

sidenote (no answer to your questions):
The bottom SMD-Pad on your footprint has the TOP-Paste and TOP-Mask-layer ticked. This happens usually if you take a TOP-SMD-Pad, copy it and than change the Copper-layer from TOP–>Bottom. But a change on the copper-pulldown-menu (in the smd-pad-properties dialog) doesn’t changes the paste/mask-layer-ticks. You have to set/unset these ticks manually.
To get a smd-pad from TOP-layer to bottom-layer (or the other way) you can also use the flip-command (hotkey “F”), this changes copper-layer and paste/mask-layer simultaneously.

sidenote2: you should set the Pad-number from the THT-Pad also to 1 == Pad-number from the SMD-Pads. Otherwise you will get drc-error later in the board-editor. (something like clearance-violation)

sidenote3: I’m not familiar with imperial thread sizes, but a hole-size of 1,4mm seems very small for a 6-32 bolt (according to your comments).

[jmk]

@Douglas777

Why not just a mounting hole and a suitable keep out area?

[Douglas777]

@paulvdh
I was just wondering if the F.Mask sufficiently implies how a stencil would be made, rather than having to explicitly also specify where the paste would go.
So, you are saying that both F.Mask and F.Paste must both be ticked for a stencil aperture to occur?
[Obviously, it would make no sense to have F.Paste ticked whilst F.Mask is unchecked!]

This bracket looks like it’s going to be screwed to the PCB.
Yes, that makes sense - there is no point in having messy solder paste where there is no intention to solder!
[Maybe that answers the query in the previous paragraph?!]

The other face of the bracket attaches to the inside of a PCB-based front panel.
To avoid a through-bolt, I can presumably solder the bracket (especially if it is made of brass, as it is).
Since the PCB is heavy and includes 200V (!), I probably need to also add blobs of epoxy.
Although soldering will likely be involved, this would be a manual process so defining the F.Paste is hardly necessary!
By soldering, rather than only using epoxy, I can achieve a tie between the front panel “chassis” (i.e., PCB-panel ground planes) and the main PCB, with the rear panel “chassis” also being connected via the PCB.
[It is a 6U module that goes into an industrial rack.]

I don’t understand this “aperture pad” subject - I would need to investigate that further …

[Douglas777]

@mf_ibfeew

Yes, I was doing this late at night after a long day …
I copied/ pasted and now realise that subsequent changes were necessary.

Regarding the hole size, it is probably something like a minimum of 3.5 mm dia that is needed.

[Douglas777]

@jmk

As explained in my reply to @paulvdh, I am trying to tie the “chassis” of the front PCB-based panel to the main PCB (which is perpendicular to it).
Also to tie the rear backplane panel “chassis” to the main PCB.

Of course, I could use a hole and add ground fill on the PCB after placing the bracket.

I am concerned about possible grounding issues.
The design is for a DC motor servo driver operating at 200V DC and up to 30 amps.
The ground of the 200V supply can be considered as “star ground”.
By “chassis” ground, I mean the ground of the PCB-based front and rear panels.

“Chassis” can also be considered as being the same as what could be referred to as “cabinet ground” of the industrial rack into which the unit slides.

There will be a dedicated external connection cable (from the machine system “earth” to the rear backplane panel “chassis”, whilst there may also be connections (of dubious electrical quality in relation to where the front panel seats against the metal racking at the top and bottom of the 6U module (assuming I provide copper in the areas - whether or not I should do is an open topic).

Of course, the front PCB needs to connect back to “earth” from a safety (and possibly also a shielding) perspective.
The machine system “earth” cable will connect to “chassis” ground via the rear PCB-based backplane.

In relation to the brackets, they provide the link from the front PCB-based panel to the main PCB.
The large pads associated with each of the two brackets (to be located near the top and bottom of the front panel) will be connected together on the main PCB and be routed in some way back as a single connection to the “star ground”.
Probably, I should only connect “chassis” to “star ground” at a single point, i.e., where the motor sinks its current?

From that “star ground” there will be other grounds radiating outwards, such as that for the 3.3V digital supply.
Possibly the main ground plane of the PCB will be such that it only connects to “star ground” at a single point (as for “chassis”)?
In other words, “chassis” ground will not be the main ground of the PCB but instead be simply routed back to the “star ground” point.

Those are my thoughts at the present time … !

The photo illustrates the general format of the product - this is an old analogue-based servo driver and I am attempting to achieve the same functionality for a new digital-based version.

[jmk]

@Douglas777

As explained in my reply to @paulvdh

I didn’t realize its purpose. I thought it was a mechanical mounting only. Thank you for explaining.

[paulvdh]

@Douglas777

@paulvdh
I was just wondering if the F.Mask sufficiently implies how a stencil would be made, rather than having to explicitly also specify where the paste would go.

KiCad does not make assumptions in this area. The things you draw in the PCB editor will be directly exported to the Gerber files, and your PCB manufacturer makes PCB’s and Stencils from them. If you have any doubt about what ends up where, then generate a set of Gerber files and view them in a Gerber viewer.

About Aperture pads: TQFP-52-1EP_10x10mm_P0.65mm_EP6.5x6.5mm is an example.
This package has a quite big GND pad in the center. If that was filled with paste, then the chip would float too high on a big blob of solder, and it’s pins won’t solder properly. Therefore the big pad (Nr 53) in the center does not have a cutout in the solder paste layer, but instead it has a lot of smaller aperture pads, which divide the required amount of solder over this pad, and also form ridges that both prevent the squeegee from dipping into this pad and scooping up solder, and the ridges also prevent air bubbles getting trapped under the IC. It’s a footprint from a default library, so you can load it in the footprint editor to examine it in more detail.

Also:
If you want pads for mechanical things then put a bunch of via’s though the pad. This makes the adherence between the PCB and the pad a lot stronger.

[straubm]

@Douglas777

I was just wondering if the F.Mask sufficiently implies how a stencil would be made

AFAIK stencils are made from the x.Paste layers.

[paulvdh]

I’ll parrot again. It’s easy from behind a keyboard:

@paulvdh

F.Mask is for the solder mask, which is the (usually green) paint on your PCB.
F.Paste is for the solder paste, which is the tacky grey stuff with solder balls and flux and these end up as the holes in the stencil.

[straubm]

So stencils are made based on x.Paste. What’s wrong with my statement??

[paulvdh]

Absolutely nothing wrong with your statement.
Just wondering why Douglas777 did not realize that the first few times he read it.
I’ll guess this is enough to get through.

[straubm]

Humans tend to be fixated on their problem and tend to mask out information.

[eelik]

Should I then copy and paste it here…