How to have copper fill include mounting holes

[Douglas777]

I am wondering how to achieve a copper fill which encompasses the positions of component mounting holes?

As illustrated, the 32-way connector has 2 mounting holes (seen in cyan) which are electrically not connected to anything.

The 3-way screw terminal black has three holes (also seen in cyan) which are provided for stubs which assist mechanical security of the component.

Since none of these cyan holes are connected to anything, I should prefer that the copper fill disregards the holes and only respects clearances from the copper pads of the components.

The cyan holes are defined as NPTH in the component footprints.

Changing the ‘Pad connection’ in ‘Clearance Overides and Settings’ (e.g., to ‘None’) does not appear to have an influence on this issue.

A second question is:
The fill’s clearance is defined as 3mm.
This seems to result in clearance of the copper fill by that amount from both the component pads and from the edges of the PCB.

How to achieve a different clearance from the PCB edge (e.g., 1mm) compared to that from the component pads?

[paulvdh]

NPTH stands for “Non Plated Through Hole”.
Your Connection to Copper Zones / Pad Connection is set to None and greyed out because it has no copper, so there is nothing that it can connect to.

@Douglas777

Since none of these cyan holes are connected to anything,

How can a hole be "connected to anything?
A hole is an absense of matter surrounded by matter.

One way to do it is to edit your footprint in the footprint editor, and then change these NPT-Holes to THT pads. You also have to give them a pad number, and add the corresponding number to the schematic symbol and add it to the appropriate net.

As an example, you can for example study:

DSUB-9_Female_Horizontal_P2.77x2.84mm_EdgePinOffset4.94mm_Housed_MountingHolesOffset7.48mm

That footprint has two holes which are defined as regular THT pads (pad number 0).

[Douglas777]

It seems that my posting has been misunderstood?

I am not wanting the (cyan) holes to be connected to anything!
Equally, I want the fill (grey colour) to disregard the holes, which as you indicate are “the absence of matter”.
i.e., I want fill to come up to the circumference of simple holes and only respect the clearance distance from copper elements such as the connector pads.

I want the holes to be simply “the absence of matter” with no associated copper.

I suppose that a possible work around would be to implement the holes as copper pads (either with or without through plating) and then associate the hole pads with a net of the same name as the fill.
Since the holes are not otherwise connected to anything else, that may achieve the same end result.

However, surely there is a way to implement a simple hole (“the absence of matter”) and have a fill disregard it in relation to clearance (but not to cover the actual hole itself).

[mf_ibfeew]

In v6 there is no standard way to get the copper directly until the hole (without tricks), there is always the edge.cuts<->copper clearance.

Regarding the original second question:

The fill’s clearance is defined as 3mm. This seems to result in clearance of the copper fill by that amount from both the component pads and from the edges of the PCB. How to achieve a different clearance from the PCB edge (e.g., 1mm) compared to that from the component pads?

You have to utilize the in v6 new introduced very mighty (but also complex/difficult) custom drc-rules-system.
Go to board-setup–>Design-rules–>Custom-rules and write your own rules. Some examples are shown upon clicking the “syntax help”-button.

For your special question:

• first you have to name your zone (zone-properties–>general–>zone name: EXAMPLE_GND_ZONE
• than you can try the following custom rule, which sets clearance between zone<–> board-edge to 0.5mm:

(version 1)
(rule “Clearance zone to board-edge”
(constraint clearance (min 0.5mm))
(condition “A.Type ==‘Zone’ && A.Name ==‘EXAMPLE_GND_ZONE’ && B.Layer ==‘Edge.Cuts’”))

[eelik]

Your board manufacturer probably doesn’t like drilling copper for a non-plated hole. Depending on how you would solve your problem in your design, which manufacturer you use and on the phase of the moon and stars, they may either make it plated or apply their minimum copper/hole distance around the hole. The solution is to apply a proper distance yourself in the design, or make it normally plated.

In any case you don’t need the copper to reach the hole edge; the problem is to apply a smaller clearance, narrower than in your screenshot.

If the mounting holes are for plastic stubs, there’s no problem in having them plated and connected to (for example) the ground fill.

[Douglas777]

Following eelik’s comments, I have changed the 3-way screw connector such that its three plastic mounting stubs are “Through-hole” (rather than “NPTH”).
I also changed the corresponding symbol such that it has three extra ‘connections’ which I have tied to “Chassis” (name of the net associated with the grey copper fill).

This results in the fill flowing around the holes for the mounting stubs.
I had to reduce the clearance to 2mm to better see the effect.
Even with that reduced clearance, the fill only surrounds the upper part of the 3 holes since the spacing of the fill has to respect clearance from the 3 pins.
I need something like the 2 or 3mm clearance since the connections are R, S and T of 3-phase electricity!

So, for this application, it can easily be concluded that no practical benefit has been gained!

The mounting pads seen at the left use a similar approach in which they are tied to the same net.

I have yet to deal with the cyan mounting hole associated with the 32-way connector.
A similar approach can be used.

Regarding my second question, I have yet to try the customs rule approach proposed by mf_ibfeew

As a third question, I am wondering if there is any drawback in having overlapping filled zones (obviously I am talking about zones associated with the same net!).
In other words, rather than trying to define a complicated polygonal shape, is it just as good to implement as overlapping rectangles?

As a fourth question, is it okay to have the copper pad of a mounting hole partly overlapping the edge cut of a PCB?
Would that cause issues with the PCB manufacturer?

Thanks to all for your assistance!

[mf_ibfeew]

As a third question, I am wondering if there is any drawback in having overlapping filled zones (obviously I am talking about zones associated with the same net!). In other words, rather than trying to define a complicated polygonal shape, is it just as good to implement as overlapping rectangles?

No big drawbacks. You can use both approaches (complicated zone versus multiple overlapping small zones). You can also first draw some simple zones and afterwards use the “context-menu → zones–> merge zones” to create the complicated zone.

As a fourth question, is it okay to have the copper pad of a mounting hole partly overlapping the edge cut of a PCB? Would that cause issues with the PCB manufacturer?

That is bad design. It may cause issues with the PCB manufacturer, but that depends (on the manufacturer). Try to avoid such situation.

[Douglas777]

My third question was:
I am wondering if there is any drawback in having overlapping filled zones (obviously I am talking about zones associated with the same net!).
In other words, rather than trying to define a complicated polygonal shape, is it just as good to implement as several overlapping rectangles?

I attach 3 graphics to provide a concrete example of what I am trying to do:

A fifth question:
I am unable to see the tracks which I have implemented (T, S, R, etc.) in the 3D view.
Is there any way to suppress the green photo resist so that I can better visualise things?

Equally, the two shades of green are very similar for both the unfilled and filled-with-copper areas.
Is there any way to change the colours?

Any general ideas/ comments relating to what I am trying to do would be much appreciated!

This is the proposed backplane for an industrial machine controller board that goes into a 19-inch rack.

The 2x 32-way DIN 41612 connectors are on the inside and all the other connectors (several screw connectors, 9-pin D-connector for RS485 and 14-pin header for programming the microcontroller) are on the rear, i.e., accessible from the outside for making connections of inputs and outputs to the system.

This is an industrial system which involves an unpleasant mix of voltages with presumably the potential for interference …

The J2 32-way DIN 41612 connector has the nasty high voltage stuff … : R, S, T 3-phase mains input, 200V DC motor output, …

In contrast, the J1 32-way DIN 41612 connector has generally lower voltages associated with it …

Approaches for shielding and earthing are subjects on which everybody will, no doubt, have different ideas!

My thinking is that, to some extent, the backplane should be considered as being an extension of the metal enclosure.
So, I propose to have the “Chassis” copper fill (seen in grey colour) on the outside face of the (proposed 2-layer) PCB.
The 6 mounting screws will tie this “Chassis” to the system chassis.

Around the J1 32-way DIN 41612 connector (i.e., the “lower-voltage” connector), I may instead use a different ground plane, i.e., the system’s digital 0v.
Going to that connector are inputs such as a +/-10V analogue signal representing the commanded speed of the motor, a signal from the system’s tachometer (indicating actual speed of the motor), various status signals from the machine, etc…

My thinking is that “chassis” and “digital ground” are best only tied together at a single place (to avoid potential hum loops, etc.)

Does my approach seem generally reasonable?!

[eelik]

@Douglas777

Is there any way to suppress the green photo resist so that I can better visualise things?

Haven’t you tried Preferences?

[Douglas777]

Thanks, the ‘Preferences’ seems to provide many useful alternatives for the 3D view.

However, the board seems to be translucent - the copper fill on the outside is also partly seen from the inside.
Is there any way to turn that translucency ‘feature’ on/ off?

[eelik]

In the same place. Double click the color; there’s an opacity setting.

[Douglas777]

I don’t see the possibility to access an opacity setting.
Are we looking at the same place?

[paulvdh]

Apparently not all items have an opacity setting.
When I open the color picker for one of the PCB layers, there is an Opacity slider on the right side:

[Frederik]

eelik wrote:
Depending on how you would solve your problem in your design, which manufacturer you use and on the phase of the moon and stars, they may either make it plated or apply their minimum copper/hole distance around the hole.

This is not quite correct. Stars do not have phases. It is the alignment of Jupiter and Saturn that affect the outcome.

[Douglas777]

In reply to:

As a third question, I am wondering if there is any drawback in having overlapping filled zones (obviously I am talking about zones associated with the same net!).
In other words, rather than trying to define a complicated polygonal shape, is it just as good to implement as overlapping rectangles?

mf_ibfeew wrote:

No big drawbacks. You can use both approaches (complicated zone versus multiple overlapping small zones).
You can also first draw some simple zones and afterwards use the “context-menu → zones–> merge zones” to create the complicated zone.

As illustrated in the following graphic, “Merge Zones” is greyed out.

That illustrates the situation when only a single zone is selected.

By holding Shift whilst clicking on the other zones to select them all, then right clicking, a different menu is seen which doesn’t have anything about zones as any of the then available menu options.

Am I doing something wrong?!

By giving each of the zones the same name (“Chassis” in my example), they all respond in the same way to the custom rule for edge clearance as was proposed by mf_ibfeew.
In that sense, they, in effect, behave as one.
Nevertheless, a more elegant solution would be to combine all into a single polygon if that is possible?

[mf_ibfeew]

Am I doing something wrong?!

Yes. I suppose you have selected not only zones but additionally some other items. For a mix of selected items (zones+tracks+vias+footprint+…) the zones-merge-command is not shown.
3 hints:

• if you try to discover a new feature or you want to use a new feature for the first time: take an almost empty project/board/schematic for this trial/learning-activity. This increases the chance that the feature works instantly. (writing a forum-post takes 5 minutes - so it’s worth to play 5 minutes prior with kicad to resolve the issue)
• play with the selection-filter on the bottom right of the screen. If you only select “zones” no other items get selected and disturb your selection. So you can easily use a box-selection-move to select all your zones.
• If you create a selection of items (for instance you want to select 3 zones in your design) the status-bar shows a sum of selected items (bottom left corner). So you can check if you have correctly selected only 3 zones or accidentally selected additionally items.

Nevertheless, a more elegant solution would be to combine all into a single polygon if that is possible?

Yes, it’s possible with the already mentioned merge zones command. Look at the attached picture:

Attention for first-time “Merge Zones”-users:

• if the zones own different properties (layer, zone-names, electrical properties, …) the properties for the merged zone are taken from one of the source-zones. It’s up to the user to check wether all properties are correct after the merge!

[Douglas777]

Returning to my original first question:

Previously I wrote:

Following eelik’s comments, I have changed the 3-way screw connector such that its three plastic mounting stubs are “Through-hole” (rather than “NPTH”).
I also changed the corresponding symbol such that it has three extra ‘connections’ which I have tied to “Chassis” (name of the net associated with the grey copper fill).

This results in the fill flowing around the holes for the mounting stubs.

Although this approach achieves the desired result, it seems very clumsy and convoluted!
I had to hack both the symbol and footprint to define the plastic stubs as if they were metallic pins and ‘electrically’ connect them to the net name of the fill in the schematic.
So changes to everything just to allow fill to go up to the perimeters of the holes …

I am wondering if there is a custom rule that could be used similar to that which overwrote the edge clearance at the board perimeter?

Could I go back to the mounting stubs being as originally defined as being “NPTH” - which is simply holes, i.e., being the ‘absence of matter’,
with a custom rule that results in the copper file extending up to that ‘absence of matter’, i.e., the perimeter of the holes, possibly with a small defined clearance in the rule (as is the case for the PCB edge rule)?

I am not wanting the fill to cover the physical hole - so no “drilling copper for a non-plated hole” is necessary

• so neither “phase of the moon and stars” or “alignment of Jupiter and Saturn” should have any effect?!

I am keen to find a more elegant solution which does not involve having to pretend that plastic pins are electrically connected to the circuit!

[Douglas777]

Thanks! Yes that works.
For others following this thread, (as you suggest) I highly recommend using the Selection filter in the bottom RH corner of screen.
In that way it can be ensured that only zones are selectable - otherwise, it is difficult to know what is being selected …

Three lines are shown at the upper border for the merged row.

How can that be simplified into a single line?
It seems to be only possible to select the complete perimeter and impractical to delete/ redo a segment to reduce surplus vertices.

Same issue at the RHS where the boundary should be definable as a single vertical line.

[paulvdh]

I am wondering why the clearance around a NPTH is so big, and whether this is a setting that got missed by Douglas777, or if it’s a missing thing or bug in KiCad.

I’m currently lacking concentration to dive deep into this though.

[mf_ibfeew]

How can that be simplified into a single line? It seems to be only possible to select the complete perimeter and impractical to delete/ redo a segment to reduce surplus vertices.

No. It’s possible with: selecting the zone (zone shows all grabbing-points and grabbing-handles), hover mouse pointer over corner points (square symbol), RMB-click–>context-menu–>remove corner