开云体育

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

I put all mounting holes also to schematic and assign appropriate mounting hole footprint to them.

开云体育

Thanks, Brian. I can select, but I see no way to mark them 'not in schematic'. I tried short-cut E, but I suppose I should use another shortcut, but which?

Select them and Mark not in schematic as a property.

On Wed, Aug 28, 2024, 2:27?PM John Woodgate via <jmw=[email protected]> wrote:

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

Thank you. I will? try that.

I put all mounting holes also to schematic and assign appropriate mounting hole footprint to them.

On K, aug 28, 2024 at 21:45, brian

<brian@...> wrote:

Select them and Mark not in schematic as a property.

On Wed, Aug 28, 2024, 2:27?PM John Woodgate via <jmw=[email protected]> wrote:

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

But, presumably John does want them in his schematic. I always include mounting holes, and have a bunch of footprints for different types.

--

开云体育

There is now a Mounting Hole Library. I don't think there was one in version 6.

But, presumably John does want them in his schematic. I always include mounting holes, and have a bunch of footprints for different types.

--

Regards,
Tony

On 28/08/2024 20:44, brian wrote:

Select them and Mark not in schematic as a property.

On Wed, Aug 28, 2024, 2:27?PM John Woodgate via <jmw=[email protected]> wrote:

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

It sounds like they have not been annotated.

Do the mounting holes exist in your schematic, or did you just try to add them onto the PCB? If the latter, that's why the reference hasn't been updated: it's because they are not in the netlist. If you double-click on the mounting hole (in pcb), you will get the footprint properties dialogue; just manually change REF** to something like MP1, MP2, MP3, etc. "Update from schematic" will always tell you they aren't used because they aren't in the schematic. I have a personal "Mounting_Point" library with schematic symbols for holes and mounting points, with and without grounding connections. That's your issue - there is no mounting point or hole schematic symbol that I can see in the standard schematic symbol libraries.

开云体育

The mounting holes are not in the schematic, any more than the mounting holes for the potentiometer are. Those mounting holes have pads, of course and are called MH1 and MH2. But I see no way of changing the 'REF**' text for the mounting holes in the PCB. In the Pad Properties pane, the Pad Type is NPTH mechanical and the Pad number field is greyed out.

There are footprints for Mounting holes, but no symbols. That seems to indicate that symbols are not required.

It sounds like they have not been annotated.

Do the mounting holes exist in your schematic, or did you just try to add them onto the PCB? If the latter, that's why the reference hasn't been updated: it's because they are not in the netlist. If you double-click on the mounting hole (in pcb), you will get the footprint properties dialogue; just manually change REF** to something like MP1, MP2, MP3, etc. "Update from schematic" will always tell you they aren't used because they aren't in the schematic. I have a personal "Mounting_Point" library with schematic symbols for holes and mounting points, with and without grounding connections. That's your issue - there is no mounting point or hole schematic symbol that I can see in the standard schematic symbol libraries.

--
Regards,
Tony

On 28/08/2024 20:44, brian wrote:

Select them and Mark not in schematic as a property.

On Wed, Aug 28, 2024, 2:27?PM John Woodgate via <jmw=[email protected]> wrote:

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Ho John,
the problem is that you are doing it wrong. Mounting holes are components, not pads. So you need to click on the component properties, and uncheck the "visible" flag on the "reference" field. I hope this helps.

开云体育

Thank you. I will try that.

Ho John,
the problem is that you are doing it wrong. Mounting holes are components, not pads. So you need to click on the component properties, and uncheck the "visible" flag on the "reference" field. I hope this helps.

Il gio 29 ago 2024, 00:43 John Woodgate via <jmw=[email protected]> ha scritto:

The mounting holes are not in the schematic, any more than the mounting holes for the potentiometer are. Those mounting holes have pads, of course and are called MH1 and MH2. But I see no way of changing the 'REF**' text for the mounting holes in the PCB. In the Pad Properties pane, the Pad Type is NPTH mechanical and the Pad number field is greyed out.

There are footprints for Mounting holes, but no symbols. That seems to indicate that symbols are not required.

On 2024-08-28 22:42, Tony Casey wrote:

It sounds like they have not been annotated.

Do the mounting holes exist in your schematic, or did you just try to add them onto the PCB? If the latter, that's why the reference hasn't been updated: it's because they are not in the netlist. If you double-click on the mounting hole (in pcb), you will get the footprint properties dialogue; just manually change REF** to something like MP1, MP2, MP3, etc. "Update from schematic" will always tell you they aren't used because they aren't in the schematic. I have a personal "Mounting_Point" library with schematic symbols for holes and mounting points, with and without grounding connections. That's your issue - there is no mounting point or hole schematic symbol that I can see in the standard schematic symbol libraries.

--
Regards,
Tony

On 28/08/2024 20:44, brian wrote:

Select them and Mark not in schematic as a property.

On Wed, Aug 28, 2024, 2:27?PM John Woodgate via <jmw=[email protected]> wrote:

I'm in trouble again. I added four mounting holes to my board and the come with? text 'REF**'. Update PCB describes them as 'unused' and proposes to delete them, which is obviously wrong. I can't find a way to change REF** to something else. Please advise.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Kicad has always understood mounting holes, and it really is very
simple. Just add them to the schematic as symbols, as others have
said. It's always been possible to make your own symbols, or make use
of something out of the supplied libraries such as a single pin
connector symbol. If you want them to relate to specific screws, put
the part number for the screw in the Value field of the schematic
symbol, and the relevant hole in the Footprint field (eg M3-HOLE). Now
when you export the BOM, it will be complete with part numbers for the
screws.

Note that by placing mounting holes in the schematic, you can optionally
connect them electrically to something, such as chassis ground
(filtering components are often connected to chassis ground rather than
signal ground). The schematic is very much the place to have the
mounting holes defined.

Regards,

Robert.

* Plain text email - safe, readable, inclusive. *

--
This email has been checked for viruses by Avast antivirus software.
www.avast.com

开云体育

Thank you. Yes, I do need to ground two of the mounting holes. These things are simple when you know how, but not if you don't. There are several steps to get exactly right.

Kicad has always understood mounting holes, and it really is very
simple.?? Just add them to the schematic as symbols, as others have
said.?? It's always been possible to make your own symbols, or make use
of something out of the supplied libraries such as a single pin
connector symbol.?? If you want them to relate to specific screws, put
the part number for the screw in the Value field of the schematic
symbol, and the relevant hole in the Footprint field (eg M3-HOLE).?? Now
when you export the BOM, it will be complete with part numbers for the
screws.

Note that by placing mounting holes in the schematic, you can optionally
connect them electrically to something, such as chassis ground
(filtering components are often connected to chassis ground rather than
signal ground).?? The schematic is very much the place to have the
mounting holes defined.

Regards,

Robert.

* Plain text email - safe, readable, inclusive. *

--
This email has been checked for viruses by Avast antivirus software.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

Exemple of how I do in schematic. Trou_fixation = Mounting hole.

开云体育

Merci.

Exemple of how I do in schematic. Trou_fixation = Mounting hole.

Regards, Jean-Paul

Site :

Le 2024-08-30 à 13:14, John Woodgate a écrit?:

Thank you. Yes, I do need to ground two of the mounting holes. These things are simple when you know how, but not if you don't. There are several steps to get exactly right.

On 2024-08-30 11:50, Robert via groups.io wrote:

Kicad has always understood mounting holes, and it really is very
simple.?? Just add them to the schematic as symbols, as others have
said.?? It's always been possible to make your own symbols, or make use
of something out of the supplied libraries such as a single pin
connector symbol.?? If you want them to relate to specific screws, put
the part number for the screw in the Value field of the schematic
symbol, and the relevant hole in the Footprint field (eg M3-HOLE).?? Now
when you export the BOM, it will be complete with part numbers for the
screws.

Note that by placing mounting holes in the schematic, you can optionally
connect them electrically to something, such as chassis ground
(filtering components are often connected to chassis ground rather than
signal ground).?? The schematic is very much the place to have the
mounting holes defined.

Regards,

Robert.

* Plain text email - safe, readable, inclusive. *

--
This email has been checked for viruses by Avast antivirus software.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Just a warning to remember to take into account creepage distance when
you have chassis ground on board. In other words, the distance between
chassis ground and all the other copper is typically greater than the
spacing used generally in order to maintain safety during faults (and
therefore electrical safety testing). For example, typically on the
boards I design I use 0.2 mm spacing, but with chassis ground (when
present) I make the spacing 0.85 mm. That way, if the internal
circuitry suddenly finds itself at a high voltage relative to chassis
ground during a fault, anyone touching the metal casing at the time wont
have their socks blown off.

Now in some respects having bolt holes connected to chassis ground in
the schematic will help you here, because in the board layout you just
make the chassis ground track spacing the relevant amount (in my case
0.85 mm), and Kicad does the rest. However, there is a gotcha. I've
not found a way to tell Kicad to maintain a safe distance /through/ the
board. That means one has to manually maintain the distance between
chassis ground and the layers beneath it ... and that's really easy to
screw up. Does anyone know a way to automate that?

Regards,

Robert.

* Plain text email - safe, readable, inclusive. *

--
This email has been checked for viruses by Avast antivirus software.
www.avast.com

开云体育

I don't agree with that, and I am involved in safety standards. Even if signal ground jumps to a high voltage due to a fault, the metal case is connected to chassis ground, which (in Class 1 equipment) is connected to the building safety ground. There is no electric shock hazard. If something has a metal case, it should be either Class 1 or Class 3 (powered by extra-low voltage). Class 2 ('double insulated') boxes should be non-conducting, even if they require an internal conductive coating or an internal foil shield for EMC reasons.

For example, typically on the
boards I design I use 0.2 mm spacing, but with chassis ground (when
present) I make the spacing 0.85 mm.?? That way, if the internal
circuitry suddenly finds itself at a high voltage relative to chassis
ground during a fault, anyone touching the metal casing at the time wont
have their socks blown off.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Don't forget that the case is connected back to the central safety earth
via a length of wire, which will have impedance.

Regards,

Robert.

--
This email has been checked for viruses by Avast antivirus software.
www.avast.com