Re: Polymide FPC ribbon cable designing

Thanks Andy,

Thank you very much for your in-depth instructions there.? I'll try to follow them this week when i get a chance.? I'm sorry for my frustration.? It's just that I HAVE used this program before, and completed three quite complicated projects in the past with it, and had total success, but other than that one transistor i had to manually modify by simply swapping two pins over, everything else has just used standard library components.? So i've never been faced with this need to go so in depth with creating or modifying a component to this degree before.? I guess it's just the frustration of wanting to "get on", but this is holding me back.? I'm going to have to spend time learning before i can get to the "heart" of the project i guess.? Hopefully i'll get there.

I'll let you know how i get on.? If i'm still struggling, i may take you up on your offer to trade emails or something so that i can maybe tap into your knowledge in a bit more of an immediate real-time affair rather than through this clunky and slow group medium...

Re: Polymide FPC ribbon cable designing

Andy Eskelson

#22344

 I'm hating this stupid program.  it's not intuitive at all!
 

 If i choose footprint libraries manager under preferences, it comes up with a hideously complicated box of complication which i don't understand at all!?Yes, that's a comment a lot of beginners make. 

It is intuitive, but like many complex tools it does take getting used to.
You are also at a slight disadvantage as a windows user. Kicad started
life as a set of Linux tools so it tends to do things the Linux way
rather than the windows way.

Kicad is not a beginners tool, and you cannot just dive into it and get
results first time, especially when doing what you want to do, which is
not a beginners project. 

Take the time to work with it, and it will click quite quickly.

The footprint libraries manager is a key part to get to know.
It's not complex it just looks as if it is. It's just two fields a
library nickname and the path to that library. 

It has a couple of tools available to append a library or a wizard to
append many.

In a big project you may have many different and specialised libraries so
knowing how to add them is pretty vital. That said it's been several
years since I've needed to add a new lib, I have about 4 additional
libs as well as a copy of the kicad libs set up and that it. Setting up
the MyConnectors library as per the previous reply was the first new lib
in several years!.

Try not to get too frustrated and shout when you get stuck. As I said
before, we have pretty much all been where you are now !

Andy

Re: Polymide FPC ribbon cable designing

Andy Eskelson

#22343

In earlier releases of Kicad, it was a bit of a pain to work with other
people on the same project, and also archive projects. Missing libs and
so on were quite common.

All the data for the components and the footprints were inside the
project, but it's not easy to deal with if you are a new the kicad.

Kicad stores all of it's data as simple text files, the cache is what
footprints you used. The components are stored directly within the .sch
files.

So if you needed to you could take the cache file, save it elsewhere, and
import that as a library.

 Over the years a lot of work has been done to make the handling of libs
 a lot easier. The first stage was to work on the footprints. if you
 see .pretty as a file extension, then that's the new format.

The next version of kicad I think has similar improvements for the
components, or if not, are planned for. I'm using the same version as
yourself, but on linux.

Kicad libs are all text file, each file containing a number of
components or footprints.

So the Connector library will hold the 1 pin, 2 pin d-type and so
on. Open a copy in notepad or a programmers editor and have a look

The key to dealing with libs is to remember that kicad will not do this
automatically. You have to tell kicad what to do and where things are.

Set up a folder somewhere in your home directory. I call mine "PCB".
In that make a directory called my-libs. In that make two directorys
called my-footprints, and my-components (or whatever you want to call
them.

To set up your first lib for footprints, open up the kicad manager,
then open pcbnew form there open up the footprint editor.

make a new footprint 6th icon on top row toolbar
give it a name say "test" then OK

Put a single pad on it somewhere. 2nd icon down on the right hand toolbar

That will do for a start.

Now select the create new library and save current footprint top toolbar
3rd icon Navigate to where you created your own directories. For a
footprint, select myFootprints and click open.

Decide what you are going to call this lib if it is a custom
set of connectors, then myConnectors will do. To the end of the library
folder path add /MyConnectors then click OK
If you look in the MyFootprints directory, you should now see another
directory called MyConnectors.pretty

That's it, the basic library is created.

close the footprint editor.

Now you just need to tell kicad to look in it.

From pcbnew, select the library management
menu > Preferences > Footprint Libraries Manager
select append library
At the bottom of the list add the library
&#92;path-to-library&#92;MyFootprints&#92;MyConnectors.pretty
Add a suitable name, in the nickname field "MyConnectors"

That should now appear in the footprint browser.
Don't worry about any error message if you see one, as the footprint with
a single pad was not complete. But do chack that the path is correct.

If you already have a number of libs from previous work, you can use
the append lib wizard to grab them all at once.

Now you can switch between your library and any other.

So open footprint editor again
select active library (top toolbar first icon)
Select Connector
Click Load footprint from library (top toolbar 8th icon)
click list all in pop up
click on BUSPCI
click OK
You should see the BUSPCI footprint displayed

Give it a slightly different name. Make sure the pointer icon top icon
right hand toolbar is active

Doubleclick on the Yellow BUSPCI text inthe footprint. a popup will
appear. Change the name to myBUSPCI click OK

Now change to your library.
Click first icon select active library (top toolbar first icon)
select myConnectors , click Ok
In the top window bar of the footprint manager you should see that your
library is now active.

Click on the save footprint in active library, top toolbar 2nd icon
Give it a name myBUSPCI if asked for.

close the footprint manager.

Now in pcbnew, select the add footprint function, click on select by
browser, select your own lib MyConnectors and you will see myBUSPCI as
an available footprint.

That's how you move footprints from one lib to another
It's much quicker to actually do than describe, and in truth you don't do
it that often Most of the time you will be working in one lib.

(Kicad now has the facilities for project specific libs as well)

Now you have the BUSPCI stored in your own lib under a different name you
can edit it to your requirements using the footprint editor

Remove the silkscreen, and chop off the pins 31 + That will be a good
start IF THE dimensions and spacings of the pins are what you need.

IF not chop out all the pins apart from pin 1 then modify the
settings via preferences Then use the array wizard to generate the other
29

Note that there are TWO pads per pin. This is in order to get the shape
needed. Any pin with the same number will join itself to others of the
same number.

Andy

On 13 Sep 2018 18:05:32 +0000
"paradox_440@... [kicad-users]" <kicad-users@...> wrote:

Okay,

 So.  I finally got to a position of peace and quiet so that i could look at Kicad again tonight.

 First off, to remind you of my two issues, and my findings for each there after.

 1.  My old project complaining about a component used not matching the entity on the database (or some other similarly worded message from 2016).  I opened up this project again.  I looked at the schematic editor and the PCB editor.  Neither made any complaints about any components this time!?  weird.  I tried a few things (not wishing to muck it up of course), like testing the schematic for errors and looking at the component in question, but nothing seemed wrong with it.  I then noticed that within the project folder where i stored everything, i have two library files.  One is called a "cache" lib and the other is called a "rescue" lib.  Both are named with the project name then "-".  So example would be "project_name-cache.lib" and "project_name-rescue.lib".  Both files are dated last edited in 2016.  Around the time i completed that project.  So i wonder if kicad is using these libraries, meaning no more error message!? - i'm guessing this isn't the best solution.

 I think i really need a step by step on libraries.  It seems i'm still confused with those.  How to set one up.  How to populate it.  How to copy existing components into it.  How to then edit components within it, and save it back there for future use.  OMG i realise how hard work i am!

 2. I looked for the suggested "BUSPCI" component.  I can find it under Run CvPcb, under connect.  But i think i need to edit this existing one first so that it simply has 30 pins and no edge cuts, which make it a PCB in its own right (is that correct?).  Otherwise i cannot assign it as the preferred footprint for an array of 30 terminals (I was looking at using "CONN_01X30" at the schematic stage - is this correct? - i DID try to use this, but i wasn't winning last weekend, so i bailed, and put in 30 individual connectors for each end of my cable schematic - so "CONN_01X01" instead)

 So with all this in mind, how do i access "BUSPCI" outside of Kicad?  I can locate the apparent "conn" entity (C:Program Files&#92;Kicad&#92;share&#92;kicad&#92;library&#92;conn.lib (and .dcm), but it doesn't give you each component separately.  So how do I set up my own personal library and copy this into it so that i can start editing it?  Perhaps once i have my own library, i can populate it with what's in the "cache" and "rescue" libraries for other projects!?  (It's made a "cache" lib within the directory of this new ribbon cable project location already!)

 I realise things may have advanced since 2016, so i thought i'd better advise of what version of Kicad i'm looking at on my laptop.  It may be old and superceded now.  I'm worried though, that if it is, and i'm advised to update it, that it messes with my other older projects and their use, since one in particular, i'm not finished with.  Life got in the way and i had to put it on a back burner so to speak.  I'd hate to disturb them or have to correct them in some way!

 So here's what i'm running:

 Version 4.0.1-stable, release build
 wxWidgets 3.0.2 Unicode and Boost 1.57.0
 Platform: Windows 8 (build 9200), 64-bit edition, 64 bit.
 (I must add that the laptop WAS Windows 8 in 2016, but it has since been upgraded to Windows 10)

 I must thank you whole heartedly for your continued patience with me!  My name is Chris by the way. :-)

Re: Symbol Creation Format

#22342

开云体育

Hi

I think I play in the 2 leagues.

I reduce the pin naming to the function in use and the name the net acording to were its connected to.

For example, a PIC pin described in the datasheet as "RC4/C3OUT/TX/CK", gets its name reduced to "RC4" and the wire (net) named "LED_1" or "LED_1_OUT".

In devices with configurble I/O like a microcontroller I simply find it too clumsy to use the full list of features on eve1ry project.

In my main library I use the full datasheet naming, but for the schematic I make a copy of the symbol to a project specific library and then adjust the pin namings to the project specific usage, and even move the pins around in order to have the inputs on the left side and the outputs to the right side.

But, thats just my way, and like in almost everything in life each one has is own preferences.

Best regards

Jorge

s 11:50 de 14/09/2018, Andy Eskelson andyyahoo@... [kicad-users] escreveu:

Show quoted text

YMMV

I find naming the pins on the device very useful.

Each project is unique, and I have no problems in creating a specific
component for each project. Like you I also name wires.

It's nice to have the choice :-)

Andy

On Fri, 14 Sep 2018 08:01:37 +0200
"'info@...' info@... [kicad-users]"
wrote:

> this will be a pita very soon as you end up using the same item over and
> over again in an new project with different functions. I always label my
> wires with their functions so i end op having named tracks on my pcb as
> well. the part itself is not changed.
>
> Simon
>
> On 14-09-18 02:19, Andy Eskelson andyyahoo@... [kicad-users] wrote:
> > The correct way is often the way that works for you.
> >
> > Devices like PLCCs are not really the same as something like a LS7400
> > where all the pins have a specific fixed functions.
> >
> > With PLCC's and uP's it makes for much better reading if the pins are
> > named for the function that they are providing for the project.
> >
> > i.e. If I use a PIC microcontroller for a project, I would grab the
> > basic component, make a copy and name the pins for what I need, such as
> > display1, 2, 3, temp-sensor1, speed-sensor etc. This makes it much easier
> > to read the circuit rather than seeing a pin that can be configured for
> > multiple functions and wondering what I decided to use it for.
> > (Especially when coming back to the design after a while)
> >
> > In the case of the 230, it would seem to make most sense to
> > group the i/o pins into the 8 pin blocks as per the datasheet and leave
> > it at that.
> >
> > The Vcc's can be grouped, as can the other few functions. You don't really
> > want to mix other functions within the general purpose i/o, that just
> > makes drawing up the circuit rather messy.
> >
> > Andy
> >
> >
> > On Thu, 13 Sep 2018 12:27:47 +0100
> > "Derek derek@... [kicad-users]" wrote:
> >
> > > Hi,
> > >
> > > I am learning how to create schematic symbols using the Component
> > Library Editor.
> > >
> > > The proces for creation of schematic symbols is easy to use. But I
> > need some advice on the format of the creation of a symbol for a Lattice
> > MACH 230.
> > >
> > > The MACH 230 is a 84 pin PLCC, which the pin connections are:
> > >
> > > 64 I/O pins
> > > 6 Vcc pins
> > > 8 GND
> > > 4 CLOCK / Input
> > > 2 Input
> > >
> > > I started out creating the smybol as detailed in the Datasheet, but
> > have read the KiCad Library Convention.
> > >
> > > Section S4.2 indicates that pins should be grouped by function.
> > >
> > > If I follow the convention, all 64 I/O pins will be grouped together.
> > >
> > > Is this the correct way to create the symbol?
> > >
> > > There are symbols availble on Github that do not follow this convention.
> > > --
> > > Regards,
> > > Derek
> >
> >
>
> --
> Met vriendelijke Groet,
>
> Simon Claessen
> drukknop.nl
>
>
> ------------------------------------
>
> ------------------------------------
>
> Please read the Kicad FAQ in the group files section before posting your question.
> Please post your bug reports here. They will be picked up by the creator of Kicad.
> Please visit for details of how to contribute your symbols/modules to the kicad library.
> For building Kicad from source and other development questions visit the kicad-devel group at
> ------------------------------------
>
> Yahoo Groups Links
>
>
>

Re: Symbol Creation Format

Andy Eskelson

#22341

YMMV

I find naming the pins on the device very useful. 

Each project is unique, and I have no problems in creating a specific
component for each project. Like you I also name wires.

It's nice to have the choice :-)

Andy

On Fri, 14 Sep 2018 08:01:37 +0200
"'info@...' info@... [kicad-users]"
<kicad-users@...> wrote:

Show quoted text

this will be a pita very soon as you end up using the same item over and 
over again in an new project with different functions. I always label my 
wires with their functions so i end op having named tracks on my pcb as 
well. the part itself is not changed.

Simon

On 14-09-18 02:19, Andy Eskelson andyyahoo@... [kicad-users] wrote:
The correct way is often the way that works for you.

Devices like PLCCs are not really the same as something like a LS7400
where all the pins have a specific fixed functions.

With PLCC's and uP's it makes for much better reading if the pins are
named for the function that they are providing for the project.

i.e. If I use a PIC microcontroller for a project, I would grab the
basic component, make a copy and name the pins for what I need, such as
display1, 2, 3, temp-sensor1, speed-sensor etc. This makes it much easier
to read the circuit rather than seeing a pin that can be configured for
multiple functions and wondering what I decided to use it for.
(Especially when coming back to the design after a while)

In the case of the 230, it would seem to make most sense to
group the i/o pins into the 8 pin blocks as per the datasheet and leave
it at that.

The Vcc's can be grouped, as can the other few functions. You don't really
want to mix other functions within the general purpose i/o, that just
makes drawing up the circuit rather messy.

Andy

On Thu, 13 Sep 2018 12:27:47 +0100
"Derek derek@... [kicad-users]" <kicad-users@...> wrote:

 > Hi,
 >
 > I am learning how to create schematic symbols using the Component   
Library Editor.  
 >
 > The proces for creation of schematic symbols is easy to use. But I   
need some advice on the format of the creation of a symbol for a Lattice 
MACH 230.  
 >
 > The MACH 230 is a 84 pin PLCC, which the pin connections are:
 >
 > 64 I/O pins
 > 6 Vcc pins
 > 8 GND
 > 4 CLOCK / Input
 > 2 Input
 >
 > I started out creating the smybol as detailed in the Datasheet, but   
have read the KiCad Library Convention.  
 >
 > Section S4.2 indicates that pins should be grouped by function.
 >
 > If I follow the convention, all 64 I/O pins will be grouped together.
 >
 > Is this the correct way to create the symbol?
 >
 > There are symbols availble on Github that do not follow this convention.
 > --
 > Regards,
 > Derek  

  -- 
Met vriendelijke Groet,

Simon Claessen
drukknop.nl

------------------------------------

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit  for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at 
------------------------------------

Yahoo Groups Links

Re: Symbol Creation Format

#22340

this will be a pita very soon as you end up using the same item over and over again in an new project with different functions. I always label my wires with their functions so i end op having named tracks on my pcb as well. the part itself is not changed.

Simon

Show quoted text

On 14-09-18 02:19, Andy Eskelson andyyahoo@... [kicad-users] wrote:
The correct way is often the way that works for you.
Devices like PLCCs are not really the same as something like a LS7400
where all the pins have a specific fixed functions.
With PLCC's and uP's it makes for much better reading if the pins are
named for the function that they are providing for the project.
i.e. If I use a PIC microcontroller for a project, I would grab the
basic component, make a copy and name the pins for what I need, such as
display1, 2, 3, temp-sensor1, speed-sensor etc. This makes it much easier
to read the circuit rather than seeing a pin that can be configured for
multiple functions and wondering what I decided to use it for.
(Especially when coming back to the design after a while)
In the case of the 230, it would seem to make most sense to
group the i/o pins into the 8 pin blocks as per the datasheet and leave
it at that.
The Vcc's can be grouped, as can the other few functions. You don't really
want to mix other functions within the general purpose i/o, that just
makes drawing up the circuit rather messy.
Andy
On Thu, 13 Sep 2018 12:27:47 +0100
"Derek derek@... [kicad-users]" <kicad-users@...> wrote:

 > Hi,
 >
 > I am learning how to create schematic symbols using the Component 
Library Editor.
 >
 > The proces for creation of schematic symbols is easy to use. But I 
need some advice on the format of the creation of a symbol for a Lattice MACH 230.
 >
 > The MACH 230 is a 84 pin PLCC, which the pin connections are:
 >
 > 64 I/O pins
 > 6 Vcc pins
 > 8 GND
 > 4 CLOCK / Input
 > 2 Input
 >
 > I started out creating the smybol as detailed in the Datasheet, but 
have read the KiCad Library Convention.
 >
 > Section S4.2 indicates that pins should be grouped by function.
 >
 > If I follow the convention, all 64 I/O pins will be grouped together.
 >
 > Is this the correct way to create the symbol?
 >
 > There are symbols availble on Github that do not follow this convention.
 > --
 > Regards,
 > Derek

-- 
Met vriendelijke Groet,

Simon Claessen
drukknop.nl

Re: Polymide FPC ribbon cable designing

Andy Eskelson

#22337

Weird, the footprint browser and the place dialogue should be looking in
exactly the same locations.

The sequence should go something like:

Open pcbnew
select add footprints (right hand toolbar 4th icon down from top)
click on board

in pop up enter:
ConnectBUSPCI

in the name box

then click OK

OR

select add footprints (right hand toolbar 4th icon down from top)
click on board
Click select by browser
 (at bottom of pop up)
click Connect in the left hand pane
click BUSPCI in the middle pane
check that it the correct footprint in the right hand pane then inser
into board by clicking on the last icon on the top menu bar.

If you sill cannot get the correct footprint email me directly and I'll
export it and you can try importing it into your setup.

Andy

On 13 Sep 2018 18:19:52 +0000
"paradox_440@... [kicad-users]" <kicad-users@...> wrote:

I also found a few FFC types under "Connectors_Molex".  I wonder if they're closer to what i'm after?  Or are they the actual connectors which the ribbon push into?  Actually i think it is.  Forget that. 

 See, i can locate "BUSPCI" under connect, but only to view from the library browser!?  Whenever i try to find it elsewhere, i can only find a hideously complicated "BUSPCI-5V".
 
 I'm struggling here.  This is all massively complicated!  It makes me wonder how on earth i fudged my way through it all 2 years ago!?
 
 Any step by step youtube videos anyone is willing to make for me to show me?

Re: Symbol Creation Format

Andy Eskelson

#22336

The correct way is often the way that works for you.

Devices like PLCCs are not really the same as something like a LS7400
where all the pins have a specific fixed functions. 

With PLCC's and uP's it makes for much better reading if the pins are
named for the function that they are providing for the project.

i.e. If I use a PIC microcontroller for a project, I would grab the
basic component, make a copy and name the pins for what I need, such as
display1, 2, 3, temp-sensor1, speed-sensor etc. This makes it much easier
to read the circuit rather than seeing a pin that can be configured for
multiple functions and wondering what I decided to use it for.
(Especially when coming back to the design after a while)
  
In the case of the 230, it would seem to make most sense to
group the i/o pins into the 8 pin blocks as per the datasheet and leave
it at that.

The Vcc's can be grouped, as can the other few functions. You don't really
want to mix other functions within the general purpose i/o, that just
makes drawing up the circuit rather messy.

Andy
 

On Thu, 13 Sep 2018 12:27:47 +0100
"Derek derek@... [kicad-users]" <kicad-users@...> wrote:

Hi,

I am learning how to create schematic symbols using the Component Library Editor.

The proces for creation of schematic symbols is easy to use. But I need some advice on the format of the creation of a symbol for a Lattice MACH 230.

The MACH 230 is a 84 pin PLCC, which the pin connections are:

64 I/O pins
6 Vcc pins
8 GND
4 CLOCK / Input
2 Input

I started out creating the smybol as detailed in the Datasheet, but have read the KiCad Library Convention.

Section S4.2 indicates that pins should be grouped by function.

If I follow the convention, all 64 I/O pins will be grouped together.

Is this the correct way to create the symbol?

There are symbols availble on Github that do not follow this convention.
-- 
Regards,
Derek

Re: Polymide FPC ribbon cable designing

#22339

Update.? Last for tonight.? I managed to open BUSPCI and start editing it, but then when it came to saving it, i couldn't!?? I couldn't set the active library because it doesn't give me the option to browse to my project folder where i managed to set up a library (i think).

when i chose "save footprint in new library", i navigated to my new project library folder and selected it.? It asked me if i was sure i wanted to overwrite this existing library.? i said yes.? Then i went to close the file and it then asked me what i wanted to do.? save and exit (why!?)? exit without save (no!)? cancel.? (no again!)

So i chose save and exit.? then i just complains that the library is not set and the footprint could not be saved.

I'm hating this stupid program.? it's not intuitive at all!

If i choose footprint libraries manager under preferences, it comes up with a hideously complicated box of complication which i don't understand at all!?

i'm getting frustrated now.? I'm having to close down my progress so far and lose it because i cant figure out how to create a library.? open an existing footprint.? edit it.? then save it in my new library.? Why is this so hard!? it's needlessly complicated!

Re: Polymide FPC ribbon cable designing

#22335

I also found a few FFC types under "Connectors_Molex".? I wonder if they're closer to what i'm after?? Or are they the actual connectors which the ribbon push into?? Actually i think it is.? Forget that.

See, i can locate "BUSPCI" under connect, but only to view from the library browser!?? Whenever i try to find it elsewhere, i can only find a hideously complicated "BUSPCI-5V".

I'm struggling here.? This is all massively complicated!? It makes me wonder how on earth i fudged my way through it all 2 years ago!?

Any step by step youtube videos anyone is willing to make for me to show me?

Re: Polymide FPC ribbon cable designing

#22338

Okay,

So.? I finally got to a position of peace and quiet so that i could look at Kicad again tonight.

First off, to remind you of my two issues, and my findings for each there after.

1.? My old project complaining about a component used not matching the entity on the database (or some other similarly worded message from 2016).? I opened up this project again.? I looked at the schematic editor and the PCB editor.? Neither made any complaints about any components this time!?? weird.? I tried a few things (not wishing to muck it up of course), like testing the schematic for errors and looking at the component in question, but nothing seemed wrong with it.? I then noticed that within the project folder where i stored everything, i have two library files.? One is called a "cache" lib and the other is called a "rescue" lib.? Both are named with the project name then "-".? So example would be "project_name-cache.lib" and "project_name-rescue.lib".? Both files are dated last edited in 2016.? Around the time i completed that project.? So i wonder if kicad is using these libraries, meaning no more error message!? - i'm guessing this isn't the best solution.

I think i really need a step by step on libraries.? It seems i'm still confused with those.? How to set one up.? How to populate it.? How to copy existing components into it.? How to then edit components within it, and save it back there for future use.? OMG i realise how hard work i am!

2. I looked for the suggested "BUSPCI" component.? I can find it under Run CvPcb, under connect.? But i think i need to edit this existing one first so that it simply has 30 pins and no edge cuts, which make it a PCB in its own right (is that correct?).? Otherwise i cannot assign it as the preferred footprint for an array of 30 terminals (I was looking at using "CONN_01X30" at the schematic stage - is this correct? - i DID try to use this, but i wasn't winning last weekend, so i bailed, and put in 30 individual connectors for each end of my cable schematic - so "CONN_01X01" instead)

So with all this in mind, how do i access "BUSPCI" outside of Kicad?? I can locate the apparent "conn" entity (C:Program Files\Kicad\share\kicad\library\conn.lib (and .dcm), but it doesn't give you each component separately.? So how do I set up my own personal library and copy this into it so that i can start editing it?? Perhaps once i have my own library, i can populate it with what's in the "cache" and "rescue" libraries for other projects!?? (It's made a "cache" lib within the directory of this new ribbon cable project location already!)

I realise things may have advanced since 2016, so i thought i'd better advise of what version of Kicad i'm looking at on my laptop.? It may be old and superceded now.? I'm worried though, that if it is, and i'm advised to update it, that it messes with my other older projects and their use, since one in particular, i'm not finished with.? Life got in the way and i had to put it on a back burner so to speak.? I'd hate to disturb them or have to correct them in some way!

So here's what i'm running:

Version 4.0.1-stable, release build

wxWidgets 3.0.2 Unicode and Boost 1.57.0

Platform: Windows 8 (build 9200), 64-bit edition, 64 bit.

(I must add that the laptop WAS Windows 8 in 2016, but it has since been upgraded to Windows 10)

I must thank you whole heartedly for your continued patience with me!? My name is Chris by the way. :-)

Symbol Creation Format

Derek

#22334

Hi,

I am learning how to create schematic symbols using the Component Library Editor.

The proces for creation of schematic symbols is easy to use. But I need some advice on the format of the creation of a symbol for a Lattice MACH 230.

The MACH 230 is a 84 pin PLCC, which the pin connections are:

64 I/O pins
6 Vcc pins
8 GND
4 CLOCK / Input
2 Input

I started out creating the smybol as detailed in the Datasheet, but have read the KiCad Library Convention.

Section S4.2 indicates that pins should be grouped by function.

If I follow the convention, all 64 I/O pins will be grouped together.

Is this the correct way to create the symbol?

There are symbols availble on Github that do not follow this convention.
--
Regards,
Derek

Re: Polymide FPC ribbon cable designing

Andy Eskelson

#22333

yes it's a lot easier with the program in front of you :-)

BUSPCI is a footprint in the connect library which should be one to the
standard libs.

there re a couple of ways to open the footprint browser
open pcbnew and then click on the third icon on the top bar, a 6 pin dil
with a mg. glass

or when you use place a footprint there is an option to browse at the
bottom of the selection window pop up.

In the browser left hand pane selects the library, select connect.
The middle pane shows the contents, and the right hand pane shows the
footprint.

Andy

On 13 Sep 2018 00:39:20 -0700
"paradox_440@... [kicad-users]" <kicad-users@...> wrote:

Ok thanks Andy. 

 I'll not admit i know all of which you speak right now, but hopefully with some time spent at the program....?
 
 Is the "BUSPCI footprint" held within Kicad already then?  Where do i find that?

Re: Polymide FPC ribbon cable designing

pierreraymondrondelle

#22332

开云体育

for your information, on page 26 of Electronics for You, Sept. 2018 there is a brief information concerning the general rules.

regards

On 13.09.18 09:39, paradox_440@... [kicad-users] wrote:

Show quoted text

?

Ok thanks Andy.

I'll not admit i know all of which you speak right now, but hopefully with some time spent at the program....?

Is the "BUSPCI footprint" held within Kicad already then?? Where do i find that?

?

Re: Polymide FPC ribbon cable designing [3 Attachments]

#22331

Ok thanks Andy.

I'll not admit i know all of which you speak right now, but hopefully with some time spent at the program....?

Is the "BUSPCI footprint" held within Kicad already then?? Where do i find that?

?

Re: Polymide FPC ribbon cable designing [3 Attachments]

Andy Eskelson

#22329

The third image shows the basic requirements.

You create a board outline using the dimensions of the cable, treat it
exactly as you would for a normal PCB outline.

For the edge connectors, load up the BUSPCI footprint and have a close
look at that. To me the form of the "fingers" look very close to what
that cable photo has. 

You then need to find out the dimensions of the fingers for that cable
and their spacing (1mm I think), then you can modify the first pad
on the BUSPCI footprint.  This has been created with TWO pads, with the
same number joined one making the main body and the other the small spike
at the end. using two pads like this is a work-around for creating pads
with more complex shapes.

(Do be careful with metric and imperial settings)
 
Adjust both to the required dimensions, and the other side pair of course.
Then you can delete all the other pads, and use the array function to
duplicate 30 pads quickly. numerate the pads. Check and then save as your
own footprint.

You can then place that at each end of the outline you create.

Tracks and so on are done exactly as normal. 

I'll have to leave it to others to explain the production process, as
it's a matter of getting the layers in the correect order...

Andy
 
On 12 Sep 2018 08:08:35 +0000
"paradox_440@... [kicad-users]" <kicad-users@...> wrote:

Hi Andy, et al. and a continued thanks.
 
 I'll need to read your instructions again as I sit at my laptop with Kicad open. I'm not even sure of the state of that particular component now, whether it's still correct or incorrect.
 
 I'll have to scratch my brain to exercise my memory as I've not looked at that project for years. It'd be good to get that component saved!
 
 As for the type of ribbon cable I want to reproduce, I've attached a photo of the actual cable I snapped (you can see the snap on the left hand end of the first photo).
 
 The Farnell link you put, is of an FFC. What I want to make is an FPC (which in my case, is just a material difference really).
 
 This is what I want to design in kicad for reproduction purposes. I hope this helps you understand what I'm trying to do. I also have a scale drawing with all dimensions on it which I drew in mspaint last week.

Re: Polymide FPC ribbon cable designing

#22328

Hi Andy, et al. and a continued thanks.

I'll need to read your instructions again as I sit at my laptop with Kicad open. I'm not even sure of the state of that particular component now, whether it's still correct or incorrect.

I'll have to scratch my brain to exercise my memory as I've not looked at that project for years. It'd be good to get that component saved!

As for the type of ribbon cable I want to reproduce, I've attached a photo of the actual cable I snapped (you can see the snap on the left hand end of the first photo).

The Farnell link you put, is of an FFC. What I want to make is an FPC (which in my case, is just a material difference really).

This is what I want to design in kicad for reproduction purposes. I hope this helps you understand what I'm trying to do. I also have a scale drawing with all dimensions on it which I drew in mspaint last week.

Re: Polymide FPC ribbon cable designing

#22327

开云体育

Hi Paradox,

?

When I read your email it brought back very familiar feelings; been there, done that.

?

KiCad is an excellent program but it's not intuitive.

?

Cheers,

Colin

Show quoted text

From: kicad-users@... [mailto:kicad-users@...]
Sent: 11 September 2018 09:04
To: kicad-users@...
Subject: [kicad-users] Re: Polymide FPC ribbon cable designing

Hi all, and thanks.

I'm a little embarrassed, but i have to admit i couldn't figure out how to edit existing templates or create new ones years ago when i last use Kicad.

I really need a youtube video or something to follow for this.? I had an issue once where i had a template for a transistor, which was perfect for what i needed for a? project one time, except two of the pins were swapped.? I managed to figure out how to swap them to the way i needed, but i couldn't save this as a new template (for whatever reason).? This meant I couldn't turn off my laptop until I had completed my entire project and saved the Gerber file i needed to send to China for manufacture!? It was a nightmare.? I actually had to go through the manufacturing process TWICE, because I didn't realise this the first time and when i was turning off my laptop and then turning it on again, the component footprint was swapping itself back the wrong way when i thought I was saving it ok!? The wrong design was sent to China, manufactured and i received it back.? It wasn't until i was soldering it up that i realised something wasn't correct!??

So every time i open that project now, Kicad? complains, telling me that footprints don't match and what do i want to do about it.? I had to edit that one component every time I opened up the project.? Nightmare!? I still never figured out how to fix this situation!

If someone could do a simple to follow video for a novice like me to watch and follow, it would be a lot of help.? I've never figured it out yet.

So to clarify.? It's a flat Polymide style 30-pin ribbon cable i need to design for manufacture.? Like this one here:

https://goo.gl/images/7ffZKz

So basically, an array of 30 flat solder pad type pins on each end of the cable, connected by lengths of printed circuitry on the cable.? It's not the connector i need, it's the thing which connects INTO the PCB mounted connector and locks into place at each end.? It's for joining circuitry together from a motherboard to a daughterboard.? I had an accident with the original, whereby it got snapped in half (they're very fragile!) and you just can't get them for love nor money.? So i'm having to make my own to replace the one i broke!

Re: Kicad version 3

#22326

It took me long enough to reply didn't it.

Thank you,? that is what I was looking for. My projects are much smaller than business cards, so I can limit the eeschema to two ground pads allowing pcbnew to create a ground plane.

Version 5 is installed on a game computer when putting lines on the silkscreen starting from both ends and trying to meet in the middle then trace over on foil levels doesn't work. That project required joining a microprocessor to a 40 pad card edge. Vertical traces on the front. Lateral traces on the back. Most lines went to two areas of the card edge with different pad sequence.

Hope the industry does not do a "Windows" and accept only updated Gerber files generated by the latest PCB software.

Hugh

On Friday, April 27, 2018, 5:55:11 a.m. MDT, 'Kaskalis T.H.' kaskalis@... [kicad-users] wrote:

Hello,

Please consider this link, also:

Regards,

Theodore

2018-04-27 11:24 GMT+03:00 Pedro Martin pkicad@... [kicad-users] <kicad-users@...>:

Show quoted text

Hi,

I have this version:
kicad-2013-07-07-BZR4022- stable-UBUNTU_12.04_full_with_ components_doc.tgz

in my computer. If you want, I can send you the file via dropbox.
It's a 267,7 MiB file.

I have also found a windows link:

I must say I have not tried this site.

Regards,
Pedro.

El 27/04/18 a las 02:20, Andy Eskelson andyyahoo@...
[kicad-users] escribi???:
>
>
> 279596318 Apr 25 2013
> kicad-2013-03-31-BZR4008- stable-UBUNTU_12.04_full_with_ components_doc.tgz
>
> On 26 Apr 2018 14:52:52 +0000 "alberta_1905@... [kicad-users]"
> <kicad-users@...> wrote:
>
> i found this via the wayback machine
>
>
>
> (Thats BZR3256)
>
> I have BZR4008 in my archives linux version
>
> 279596318 Apr 25 2013
> kicad-2013-03-31-BZR4008- stable-UBUNTU_12.04_full_with_ components_doc.tgz
>
> Andy
>
>> What happened to Kicad Old Stable? Even search engines refuse to list
> anything before version 4.0.
>>
>>
>> Hugh
>>
>
>

------------------------------ ------

------------------------------ ------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at
------------------------------ ------

Yahoo Groups Links

<*> To visit your group on the web, go to:
? ?

<*> Your email settings:
? ? Individual Email | Traditional

<*> To change settings online go to:
? ?
? ? (Yahoo! ID required)

<*> To change settings via email:
? ? kicad-users-digest@ yahoogroups.com
? ? kicad-users-fullfeatured@ yahoogroups.com

<*> To unsubscribe from this group, send an email to:
? ? kicad-users-unsubscribe@ yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
? ?

Re: Polymide FPC ribbon cable designing

Andy Eskelson

#22325

Ok there are a couple of issues here. You are talking about a ribbon
cable, however what the replies are all about are flexible PCB's which is
what the image you posed is.

Before you go too far along this path. Is this what you are looking for: 

The interconnect style ribbons are widely available is various sizes and
are quite cheap, the above one is a molex 0.5mm pitch 30 way 0.152m long
2 UKP if this will fit your requirements it will save a lot of
work. 

Editing either components or footprints in kicad is slightly different to
some other software, as it involves things stored in multiple libraries 

First, be very careful in how you describe and think of things. In kicad
your have components that you place on the circuit diagram using
eeschema, and then you have footprints that you place on the PCB with
Pcbnew. The pin numbering / id's on the two must match for the
connection to be made. 

What is happening in your project is that you have edited either the
footprint or the component to fix the issue, but failed to save the
change. A common issue.

Both the schematic library editor, and the footprint editor work in a
similar way. I'll describe the setup for the footprint editor. Note that
I am using kicad 4 at the moment.

Open the footprint editor and look at the top icon bar

The first three icons are key

The first is select active library 
This tells the editor where to look for the footprint you want to work
on, and makes that library active.

The second icon is save the footprint in the active library
Does what it says, but you HAVE to select the library with the first icon
first.

The third icon is useful to set up your own libs.
Make a new footprint, it can be a single pad if you wish :-) then click
on the third icon, select the base path give it a name then OK 
Job done.

After that you can then use the first icon to select that library when
you want to edit things in it.

When you edit a footprint then save it, if the footprint exists in the
library you will get a warning. Either save and overwrite or not.

If you want to modify a footprint, select the library that the footprint
is in, load it, then make your changes.

Note that during the creation / editing of the footprint, the VALUE field
is used as the name of the footprint. That little oddity confused me at
first :-) Make sure you use a different name if you want/need to keep
the origional

Then select the library you want the module to be saved in (say your own
library) then click the save in active library ALWAYS check the top of
the footprint window title bar, that tells you what the current active
library is.

That's the main "trick" to editing and creating things with kicad, the
other icons are pretty much self explanatory. For editing, the properties
setting is the main thing you will use, as I mentioned the pin number
and pad numbers need to match.

Once you have modified and saved the footprint into a library (usually
your own if you want to avoid things changing)  

Open your project, and make sure you have added the library where the new
footprint is saved. then you can edit the component on the circuit
diagram (use properties) and then select the new footprint.

You can also do much the same thing with Pcbnew select the footprint,
then properties then change footprint.

Shout if you get stuck and need a bit of help. We all went through this
at first!

Andy
 
On 11 Sep 2018 08:04:19 +0000
"paradox_440@... [kicad-users]" <kicad-users@...> wrote:

Hi all, and thanks.
 
 I'm a little embarrassed, but i have to admit i couldn't figure out how to edit existing templates or create new ones years ago when i last use Kicad.
 
 I really need a youtube video or something to follow for this.  I had an issue once where i had a template for a transistor, which was perfect for what i needed for a  project one time, except two of the pins were swapped.  I managed to figure out how to swap them to the way i needed, but i couldn't save this as a new template (for whatever reason).  This meant I couldn't turn off my laptop until I had completed my entire project and saved the Gerber file i needed to send to China for manufacture!  It was a nightmare.  I actually had to go through the manufacturing process TWICE, because I didn't realise this the first time and when i was turning off my laptop and then turning it on again, the component footprint was swapping itself back the wrong way when i thought I was saving it ok!  The wrong design was sent to China, manufactured and i received it back.  It wasn't until i was soldering it up that i realised something wasn't correct!  
 So every time i open that project now, Kicad  complains, telling me that footprints don't match and what do i want to do about it.  I had to edit that one component every time I opened up the project.  Nightmare!  I still never figured out how to fix this situation!
 
 If someone could do a simple to follow video for a novice like me to watch and follow, it would be a lot of help.  I've never figured it out yet.
 
 So to clarify.  It's a flat Polymide style 30-pin ribbon cable i need to design for manufacture.  Like this one here:
 
 So basically, an array of 30 flat solder pad type pins on each end of the cable, connected by lengths of printed circuitry on the cable.  It's not the connector i need, it's the thing which connects INTO the PCB mounted connector and locks into place at each end.  It's for joining circuitry together from a motherboard to a daughterboard.  I had an accident with the original, whereby it got snapped in half (they're very fragile!) and you just can't get them for love nor money.  So i'm having to make my own to replace the one i broke!