|
Have made "hole" footprints. place in a "local hole library" - feedback insane requirement to make a footprint for holes.
Place my holes nice holes in the PCB.
Then "updated" my PCB to schematic to make sure I was not missing anything.?
?????????? Tools->Update PCB from Schematic
Placed "hole" footprints just went away.!!!!!!!
How do you keep this from happening??? -?Do you seriously have to place "hole" symbols on the schematic? There are > 200 messages about mounting holes.
What did I miss in the help manual ?
Please Oh Please enlighten me, On how to keep my mounting holes from being tossed.
|
On Tue, 12 Nov 2019 at 23:45, John <jphutch60bj@...> wrote:
Have made "hole" footprints. place in a "local hole library" - feedback insane requirement to make a footprint for holes.
Place my holes nice holes in the PCB.
Then "updated" my PCB to schematic to make sure I was not missing anything.
Tools->Update PCB from Schematic
Placed "hole" footprints just went away.!!!!!!!
How do you keep this from happening?
You select the footprint in your PCB and edit the properties. There you have a choice of "locking" the component, so it will not be be removed by an update from the schematic. -?Do you seriously have to place "hole" symbols on the schematic? There are > 200 messages about mounting holes. What did I miss in the help manual ?
Please Oh Please enlighten me, On how to keep my mounting holes from being tossed.
|
Or place a symbol to your schematic, and add the footprint to it.
On Wed, Nov 13, 2019, 09:09 Henner Zeller < h.zeller@...> wrote: On Tue, 12 Nov 2019 at 23:45, John <jphutch60bj@...> wrote:
>
> Have made "hole" footprints. place in a "local hole library" - feedback insane requirement to make a footprint for holes.
> Place my holes nice holes in the PCB.
> Then "updated" my PCB to schematic to make sure I was not missing anything.
>? ? ? ? ? ? Tools->Update PCB from Schematic
> Placed "hole" footprints just went away.!!!!!!!
> How do you keep this from happening?
You select the footprint in your PCB and edit the properties. There
you have a choice of "locking" the component, so it will not be be
removed
by an update from the schematic.
?-?Do you seriously have to place "hole" symbols on the schematic?
There are > 200 messages about mounting holes.
> What did I miss in the help manual ?
> Please Oh Please enlighten me, On how to keep my mounting holes from being tossed.
>
|
Scrivo in italiano, perché il mio inglese e' pessimo. Ma so che tanti lo potranno ugualmente leggere e capire.
A? proposito dei pads per i lavori in montaggi con fori passanti, ho dovuto fare due diverse librerie "proprietarie" per questo inconveniente. Nelle precedenti versioni di Kicad, dalla 3xxx e quindi la 4022, poi la 4.0.7, le librerie/simboli ?avevano i pads di montaggio ANCHE in serigrafia lato componenti. Per la produzione, bastava dichiarare "foratura reale" (funzione "stampa") per avere una giusta forma dei pads in serigrafia: con la 4.0.7 si avevano i pads "cerchiati" in serigrafia, ottimo sia per montaggio del prototipo, sia per la produzione. ?In produzione la serigrafia NON copriva i pads ma li indicava solamente, senza disturbare la zona di saldatura. Ora, con la 5.1.4_1, nelle librerie "proprie" di Kicad, i? pads in serigrafia lato componenti non sono presenti. Per avere la serigrafia completa ho fatto due diverse librerie-impronte: una coi pads per i prototipi in laboratorio, una senza per la produzione, perché il comando "foratura reale", nella funzione "print", "print-preview" e relativa stampa, ?funziona per la foratura al pcb,? ma non piu', come invece faceva nella 4.0.7, sulla traccia di serigrafia lato componenti.
Saluti, grazie.
Carlo Garberi.
Il mercoledì 13 novembre 2019, 08:45:16 CET, John <jphutch60bj@...> ha scritto:
Have made "hole" footprints. place in a "local hole library" - feedback insane requirement to make a footprint for holes.
Place my holes nice holes in the PCB.
Then "updated" my PCB to schematic to make sure I was not missing anything.?
?????????? Tools->Update PCB from Schematic
Placed "hole" footprints just went away.!!!!!!!
How do you keep this from happening??? -?Do you seriously have to place "hole" symbols on the schematic? There are > 200 messages about mounting holes.
What did I miss in the help manual ?
Please Oh Please enlighten me, On how to keep my mounting holes from being tossed.
|
That's what I do. And if the board profile is something complicated
that has come from a mechanical CAD application (as a DXF), I have a
"board" component that includes the holes, the profile, and anything
else I will need to know whilst laying out (such as keep-outs). The
board I'm currently working on even has solder pads for a pig-tail baked
into the board footprint.
Regards,
Robert
toggle quoted message
Show quoted text
On 13/11/2019 01:26, John wrote: Do you seriously have to place "hole" symbols on the schematic?
|
Hi Robert, can you show how it looks?like?
"The board?I'm currently working on even has solder pads for a pig-tail baked into?the board footprint."
That's what I do.? ?And if the board profile is something complicated
that has come from a mechanical CAD application (as a DXF), I have a
"board" component that includes the holes, the profile, and anything
else I will need to know whilst laying out (such as keep-outs).? ?The
board I'm currently working on even has solder pads for a pig-tail baked
into the board footprint.
Regards,
Robert
On 13/11/2019 01:26, John wrote:
> Do you seriously have to place "hole" symbols on the schematic?
|
Sure, if attaching a file to a post works on groups.io (it was rather hit-and-miss on Yahoo groups). If it doesn't work, I'll send the image direct to you. The image is confusing if you don't know what it all means. Firstly, it shows just the left-hand end of the board. The green and the yellow lines are on the eco1 and eco2 layers, used to show me where are the keep-out areas on either side of the board. The outer green line overlays the board profile, so you can't see the lines on the profile layer, but they're there, baked into the footprint. The purple text is on the silk screen. The items in grey (the drawings layer) show me where one of the other engineers wants me to place items that have to be in a specific position, including the pig-tail pads (I just have to remember which side of the board they are on). 1 to 9 are pads for a pig-tail, and the pads marked 10 are for bolt holes that connect electrically to the metal case. I could have made the pigtail pads a separate footprint, but it was convenient in this case to do things as I have. I could also have numbered the pads marked 10 as 9, since in this case they are connected electrically, but instead I opted to show the connection on the schematic to make it salient to people looking at the schematic. Speaking of which, this entire footprint is represented in the schematic as a ten pin connector. Sometimes I have the board as a separate component (with or without a connection to chassis); it just depends on what works best for a particular project. All the elements you see except the pads are imported from DXFs sent through from two engineers working on other aspects of the project. Regards, Robert. On 13/11/2019 09:21, José Eduardo S. C. Xavier wrote: Hi Robert, can you show how it looks like?
"The board I'm currently working on even has solder pads for a pig-tail baked
into the board footprint."
On Wed, Nov 13, 2019, 08:55 Robert <birmingham_spider@...
<mailto:birmingham_spider@...>> wrote:
That's what I do. And if the board profile is something complicated
that has come from a mechanical CAD application (as a DXF), I have a
"board" component that includes the holes, the profile, and anything
else I will need to know whilst laying out (such as keep-outs). The
board I'm currently working on even has solder pads for a pig-tail baked
into the board footprint.
Regards,
Robert
On 13/11/2019 01:26, John wrote:
> Do you seriously have to place "hole" symbols on the schematic?
-- () Plain text email - safe, readable, inclusive. /\
|
How do you specify your mounting holes in the DXF?
Levente
toggle quoted message
Show quoted text
On Wed, Nov 13, 2019 at 9:55 AM Robert <birmingham_spider@...> wrote:
That's what I do. And if the board profile is something complicated
that has come from a mechanical CAD application (as a DXF), I have a
"board" component that includes the holes, the profile, and anything
else I will need to know whilst laying out (such as keep-outs). The
board I'm currently working on even has solder pads for a pig-tail baked
into the board footprint.
Regards,
Robert
On 13/11/2019 01:26, John wrote:
Do you seriously have to place "hole" symbols on the schematic?
|
Yes it is good to add Mechanical Items on your sch if you use DXF layers you still need to add a hole Just DXF does
Not equate to Hole in Drill file. You have no Idea how many times people proudly share their work on Linkedin and have
Mounting holes
DXF is good to position a Hole but you need to put a Hole on the pcb to create a Hole in the NC Drill Slots can be done Via DXF as they are Routed
not drilled .
This is Not CAD tool related no Cad tool Creates a Hole in the NC Drill from a DXF layer.
Arie
toggle quoted message
Show quoted text
-----Original Message----- From: [email protected] < [email protected]> On Behalf Of Lev Sent: Wednesday, November 13, 2019 1:35 PM To: [email protected]Subject: Re: [kicad-users] Mounting holes disappear when updating PCB to schematic - expletive Tools->Update PCB from Schematic How do you specify your mounting holes in the DXF? Levente On Wed, Nov 13, 2019 at 9:55 AM Robert <birmingham_spider@...> wrote:
That's what I do. And if the board profile is something complicated
that has come from a mechanical CAD application (as a DXF), I have a
"board" component that includes the holes, the profile, and anything
else I will need to know whilst laying out (such as keep-outs). The
board I'm currently working on even has solder pads for a pig-tail
baked into the board footprint.
Regards,
Robert
On 13/11/2019 01:26, John wrote:
Do you seriously have to place "hole" symbols on the schematic?
|
The mechanical designer places circles in the DXF. Obviously there's a circle for the hole proper, with additional larger circles as required for the copper annulus and/or keep-out (don't forget things like the bolt head, washers, and tolerances). Having imported the DXF, I then place a pad to match. KiCad 5 helpfully snaps the pad into position, whereas previously I would have had to eyeball it (which is actually very easy). There are errors in this process, which can be reduced if one goes back to the original mechanical drawing so the hole can be positioned using measurements taken from that, with the imported DXF being used as a check. In practice I don't bother; I just feed back some sort of mechanical export from KiCad, such as STEP, and let the mechanical designer check everything fits into the 3D model of the product, because that's what actually matters, not a 2mm bolt hole being 0.001659mm off-centre. He's yet to complain about the errors, as they are insignificant. I don't know where they creep in in the chain from the original 3D model through to KiCad and back again, but they do; maybe something is going through a metric/US units conversion. Just recently we've been trying to rationalise the numbers, eg by making sure everything is a multiple of 0.1mm. That just makes it easier to spot a real problem. Regards, Robert On 13/11/2019 11:35, Lev wrote: How do you specify your mounting holes in the DXF? -- () Plain text email - safe, readable, inclusive. /\
|
Love google : Scrivo in inglese, perché il mio italiano è inesistente.? and got it translated.
1. lock down thanks - using the wrong lock down option button.
2. yes: did add holes - symbols to the schematic after writing my blurb, and finding a previous post indicating such action was needed and how to do it.
The ultimate in schematic driven layout, got to love it.
Thanks for the many replies.
Saluti, grazie. }
Hutch
|
Henner,
Using V6.0.8 here. I tried your suggestion of locking the mounting holes. Performed an update from the schematic. Mounting holes disappeared. Your suggestion to lock them was just a guess?
|
In the KiCad PCB Editor a selected component can be 'locked' with hotkey 'L' by default. I assume you are placing your mounting holes in the PCB Editor using 'Add a footprint' (hotkey 'A') and selecting a footprint from the MountingHole library (i.e. 'MountingHole_3.2mm_M3' or something). Such a component should survive an update from the schematic (using 'Update PCB from Schematic') UNLESS you have selected 'Delete footprints with no symbols'.  If you have that selected, your additional footprints will get blown away even if you locked them beforehand.
|
Hi
I do take the easy way out of such issues.
I had the mounting holes and similar features to the schematic.
NOTE:
If you don't have a mounting hole component in your symbol
libraries just had a single point connector and associate it with
a mounting hole footprint.
HIH
Best regards
Happy new year
Jorge
toggle quoted message
Show quoted text
Henner,
Using V6.0.8 here. I tried your suggestion of locking the mounting
holes. Performed an update from the schematic. Mounting holes
disappeared. Your suggestion to lock them was just a guess?
|
Hello.
I always put mounting holes also to schematics and define the footprint there. This way they won't disappear.
Br.
On L, dets 31, 2022 at 1:00, Chris via groups.io <chris.carter.iee@...> wrote: [Edited Message Follows]
In the KiCad PCB Editor a selected component can be 'locked' with hotkey 'L' by default. I assume you are placing your mounting holes in the PCB Editor using 'Add a footprint' (hotkey 'A') and selecting a footprint from the MountingHole library (i.e. 'MountingHole_3.2mm_M3' or something). Such a component should survive an update from the schematic (using 'Update PCB from Schematic') UNLESS you have selected 'Delete footprints with no symbols'.  If you have that selected, your additional footprints will get blown away even if you locked them beforehand.
|
I have not used Kicad for a while now so my answer may be dated.? I had the same problem once.? Read somewhere that I had to have the holes on the scematic page, thought it was strange, did it any way.? It worked though.? ?Simply arranged them on right of schematic and then arranged them on PCB. Tey sid not disappear again.
Have made "hole" footprints. place in a "local hole library" - feedback insane requirement to make a footprint for holes.
Place my holes nice holes in the PCB.
Then "updated" my PCB to schematic to make sure I was not missing anything.?
?????????? Tools->Update PCB from Schematic
Placed "hole" footprints just went away.!!!!!!!
How do you keep this from happening??? -?Do you seriously have to place "hole" symbols on the schematic? There are > 200 messages about mounting holes.
What did I miss in the help manual ?
Please Oh Please enlighten me, On how to keep my mounting holes from being tossed.
|
Jaak Pieterse