Mixed part types with multi-part components?

#11898

Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the parts libraries I need. This seems to be a nightmare for every program I try, like they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. The problem seems to be when I am making a component which has multiple parts, but they aren't all the same. For instance, tonight I am trying to make a big library of transistor and diode arrays that I use. Now I am trying to enter a device (THAT 340) which has two NPN transistors, and two PNP transistors. I define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for Part B, I go back and it has overwritten the PNP for PART A also! I cannot imagine any reason why this would happen. They have their own pin numbers! If I change the part for pins 5-7 why would it assume that I am changing pins 1-3 which I have already done?

The only workaround I can think of for now is just using a monolithic block and naming the pins for the whole device. It's easy, but it makes the schematics messy. Any ideas? Am I missing something here?

Thanks!

Andy Eskelson

#11901

It can be done fairly easily.
I created a relay symbol that had the coil and contacts as sep parts.

In the component properties you need to set the number of parts, I expect
that you have done this for other parts you have created.

Then you can start editing the component. In the top toolbar there are
two boxes, one to select the part A, B, C and so on. then a box for the
name. Next to that box is a button "edit pins per part or body style" 

Click this so that it is active. this setting allows you to use
different designs and pins for each sub part.

If I remember correctly there was a small problem in getting things to
edit correctly, and what I did was to just put a single line on all
parts (with the edit pins button unselected, then switch it back on and
I could then edit things as normal.  I've not tried to do this with my
current version of kicad,  BZR 3256, so that little problem may have
been sorted out by now.

Andy

 



On Thu, 12 Apr 2012 22:33:21 -0000
"acousmatique" <acousmatique@...> wrote:

Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the parts libraries I need. This seems to be a nightmare for every program I try, like they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. The problem seems to be when I am making a component which has multiple parts, but they aren't all the same. For instance, tonight I am trying to make a big library of transistor and diode arrays that I use. Now I am trying to enter a device (THAT 340) which has two NPN transistors, and two PNP transistors. I define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for Part B, I go back and it has overwritten the PNP for PART A also! I cannot imagine any reason why this would happen. They have their own pin numbers! If I change the part for pins 5-7 why would it assume that I am changing pins 1-3 which I have already done?

The only workaround I can think of for now is just using a monolithic block and naming the pins for the whole device. It's easy, but it makes the schematics messy. Any ideas? Am I missing something here?

Thanks!



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

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 ! Groups Links

#11902

well i don't know about easily:

creating same parts is not a problem.?

creating parts where pins are in different position from one part to next is not a problem

creating different artwork for each part is a problem.?

every time i change one part, change is applied to all of them.

i did try various settings incl. edit pins per part but so far this is still frustrating.

Show quoted text

From: Andy Eskelson
To: kicad-users@...
Sent: Friday, April 13, 2012 4:24:19 AM
Subject: Re: [kicad-users] Mixed part types with multi-part components?

It can be done fairly easily.
I created a relay symbol that had the coil and contacts as sep parts.

In the component properties you need to set the number of parts, I expect
that you have done this for other parts you have created.

Then you can start editing the component. In the top toolbar there are
two boxes, one to select the part A, B, C and so on. then a box for the
name. Next to that box is a button "edit pins per part or body style"

Click this so that it is active. this setting allows you to use
different designs and pins for each sub part.

If I remember correctly there was a small problem in getting things to
edit correctly, and what I did was to just put a single line on all
parts (with the edit pins button unselected, then switch it back on and
I could then edit things as normal. I've not tried to do this with my
current version of kicad, BZR 3256, so that little problem may have
been sorted out by now.

Andy

On Thu, 12 Apr 2012 22:33:21 -0000
"acousmatique" <acousmatique@...> wrote:

> Arg... this is driving me nuts.
>
> For the past two weeks, I have buckled down to create the parts libraries I need. This seems to be a nightmare for every program I try, like they assume the parts you need are already there.
>
> I have made some multi-part profiles which have turned out well. The problem seems to be when I am making a component which has multiple parts, but they aren't all the same. For instance, tonight I am trying to make a big library of transistor and diode arrays that I use. Now I am trying to enter a device (THAT 340) which has two NPN transistors, and two PNP transistors. I define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for Part B, I go back and it has overwritten the PNP for PART A also! I cannot imagine any reason why this would happen. They have their own pin numbers! If I change the part for pins 5-7 why would it assume that I am changing pins 1-3 which I have already done?
>
> The only workaround I can think of for now is just using a monolithic block and naming the pins for the whole device. It's easy, but it makes the schematics messy. Any ideas? Am I missing something here?
>
> Thanks!
>
>
>
> ------------------------------------
>
> 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 ! Groups Links
>
>
>

Andy Eskelson

#11903

That reminded me of the problem - it's obviously still the same.

I've just had a quick play and I've reminded myself of the way to do
things. It's a bit annoying but this is how to get around the problem

set things up as before, with the correct number of parts.
The edit pins per pare should normally be selected.


Now select the part you want to edit.

select a drawing tool, and click ONCE to start the tool. Then RIGHT CLICK
and select the edit rectangle/line options.

untick the shared by all parts in component button.

That should do the trick. Once set to this mode it will usually be
remembered but you do need to do this each time you start a new edit.

You can also change the setting once drawn. Select the general pointer
tool, the arrow at the top of the right hand toolbar. The RIGHT click on
a rectangle or line that will bring up a zoom / move sub menu. right
click AGAIN in the same place and you will get the rectangle / line
options from there you can select the shared on all parts button again.

(What happens is that the first click assumes that you want to zoom the
page etc)


If you have lots of lines then this is a bit tedious and it's better to
start off the process with the correct settings. However I have not found
a way to copy blocks between parts from the editor, so if you do have
some common graphics the it is sometimes easier to leave the settings as
common to all parts, then go into each part, switch off that option and
make the tweaks from there. This could do with a bit of work done on it
to make things easier...


Andy






On Fri, 13 Apr 2012 02:38:32 -0700 (PDT)
Ivica Kvasina <kvasina@...> wrote:

well i don't know about easily:
creating same parts is not a problem.?
creating parts where pins are in different position from one part to next is not a problem
creating different artwork for each part is a problem.?
every time i change one part, change is applied to all of them.
i did try various settings incl. edit pins per part but so far this is still frustrating.



________________________________
 From: Andy Eskelson <andyyahoo@...>
To: kicad-users@...
Sent: Friday, April 13, 2012 4:24:19 AM
Subject: Re: [kicad-users] Mixed part types with multi-part components?


?
It can be done fairly easily.
I created a relay symbol that had the coil and contacts as sep parts.

In the component properties you need to set the number of parts, I expect
that you have done this for other parts you have created.

Then you can start editing the component. In the top toolbar there are
two boxes, one to select the part A, B, C and so on. then a box for the
name. Next to that box is a button "edit pins per part or body style"

Click this so that it is active. this setting allows you to use
different designs and pins for each sub part.

If I remember correctly there was a small problem in getting things to
edit correctly, and what I did was to just put a single line on all
parts (with the edit pins button unselected, then switch it back on and
I could then edit things as normal.  I've not tried to do this with my
current version of kicad,  BZR 3256, so that little problem may have
been sorted out by now.

Andy

On Thu, 12 Apr 2012 22:33:21 -0000
"acousmatique" <acousmatique@...> wrote:

Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the parts libraries I need. This seems to be a nightmare for every program I try, like they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. The problem seems to be when I am making a component which has multiple parts, but they aren't all the same. For instance, tonight I am trying to make a big library of transistor and diode arrays that I use. Now I am trying to enter a device (THAT 340) which has two NPN transistors, and two PNP transistors. I define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for Part B, I go back and it has overwritten the PNP for PART A also! I cannot imagine any reason why this would happen. They have their own pin numbers! If I change the part for pins 5-7 why would it assume that I am changing pins 1-3 which I have already done?

The only workaround I can think of for now is just using a monolithic block and naming the pins for the whole device. It's easy, but it makes the schematics messy. Any ideas? Am I missing something here?

Thanks!



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

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 ! Groups Links

#11905

Ah, yes, this one had me tearing my hair out a few weeks ago.   The key to it is the button on the far right of the library editor marked with a crossed-out black pin and a red pin, "Edit pins per part or body style (Use carefully!)".   I can't remember if it has to be 'up' or 'down' to get what you want, so you'll have to try both ways :).

Regards,

Robert.

Show quoted text

On 12/04/2012 23:33, acousmatique wrote:
Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the parts
libraries I need. This seems to be a nightmare for every program I
try, like they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. The
problem seems to be when I am making a component which has multiple
parts, but they aren't all the same. For instance, tonight I am
trying to make a big library of transistor and diode arrays that I
use. Now I am trying to enter a device (THAT 340) which has two NPN
transistors, and two PNP transistors. I define pins 1-3 as NPN for
Part A, but then when I define pins 5-7 as PNP for Part B, I go back
and it has overwritten the PNP for PART A also! I cannot imagine any
reason why this would happen. They have their own pin numbers! If I
change the part for pins 5-7 why would it assume that I am changing
pins 1-3 which I have already done?

The only workaround I can think of for now is just using a monolithic
block and naming the pins for the whole device. It's easy, but it
makes the schematics messy. Any ideas? Am I missing something here?

Thanks!



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

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
! Groups Links




--- avast! Antivirus: Inbound message clean. Virus Database (VPS):
120412-1, 12/04/2012 Tested on: 13/04/2012 08:59:14 avast! -
copyright (c) 1988-2012 AVAST Software. 

-- 
() Plain text email - safe, readable, inclusive.
/&#92; 

#11907

Thanks for the helpful suggestions. I have gotten some work done by clicking the "parts are locked" box in properties. This causes each part to be locked as its own entity. But this worked only for pins, not the other shapes I needed to draw. Then I needed to fiddle with the Edit line options > Shared by all parts in component box. Flipping back and forth between parts, I clicked this box on/off a few times with some parts until the setting appeared to take. And the whole process involved more re-drawing than I wanted. But it worked and will do for now.

I will also definitely check out the "Edit pins per part or body style" button.

#12214

For the pins it work well, but with the artwork KiCAD had some problem:

On all parts it places the same artwork. I call it a bug...

Roland

Show quoted text

--- In kicad-users@..., Ivica Kvasina <kvasina@...> wrote:

well i don't know about easily:
creating same parts is not a problem.??
creating parts where pins are in different position from one part to next is not a problem
creating different artwork for each part is a problem.??
every time i change one part, change is applied to all of them.
i did try various settings incl. edit pins per part but so far this is still frustrating.



________________________________
 From: Andy Eskelson <andyyahoo@...>
To: kicad-users@...
Sent: Friday, April 13, 2012 4:24:19 AM
Subject: Re: [kicad-users] Mixed part types with multi-part components?


??
It can be done fairly easily.
I created a relay symbol that had the coil and contacts as sep parts.

In the component properties you need to set the number of parts, I expect
that you have done this for other parts you have created.

Then you can start editing the component. In the top toolbar there are
two boxes, one to select the part A, B, C and so on. then a box for the
name. Next to that box is a button "edit pins per part or body style"

Click this so that it is active. this setting allows you to use
different designs and pins for each sub part.

If I remember correctly there was a small problem in getting things to
edit correctly, and what I did was to just put a single line on all
parts (with the edit pins button unselected, then switch it back on and
I could then edit things as normal.  I've not tried to do this with my
current version of kicad,  BZR 3256, so that little problem may have
been sorted out by now.

Andy

On Thu, 12 Apr 2012 22:33:21 -0000
"acousmatique" <acousmatique@...> wrote:

Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the parts libraries I need. This seems to be a nightmare for every program I try, like they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. The problem seems to be when I am making a component which has multiple parts, but they aren't all the same. For instance, tonight I am trying to make a big library of transistor and diode arrays that I use. Now I am trying to enter a device (THAT 340) which has two NPN transistors, and two PNP transistors. I define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for Part B, I go back and it has overwritten the PNP for PART A also! I cannot imagine any reason why this would happen. They have their own pin numbers! If I change the part for pins 5-7 why would it assume that I am changing pins 1-3 which I have already done?

The only workaround I can think of for now is just using a monolithic block and naming the pins for the whole device. It's easy, but it makes the schematics messy. Any ideas? Am I missing something here?

Thanks!



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

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 ! Groups Links

#12221

Hi,

I don't know if it is a bug in the last versions, but with a 2008 version we
made some components with different parts and they work properly with
2011-07-08 version we are still using.

We have a component with 6 different parts, each of them a rectangle, but
different rectangles in size.

Regards,
Pedro.

For the pins it work well, but with the artwork KiCAD had some problem:

On all parts it places the same artwork. I call it a bug...

Roland

--- In kicad-users@..., Ivica Kvasina <kvasina@...> wrote:

well i don't know about easily:
creating same parts is not a problem.?
creating parts where pins are in different position from one part to nextis not a problem
creating different artwork for each part is a problem.?
every time i change one part, change is applied to all of them.
i did try various settings incl. edit pins per part but so far this isstill frustrating.



________________________________
 From: Andy Eskelson <andyyahoo@...>
To: kicad-users@...
Sent: Friday, April 13, 2012 4:24:19 AM
Subject: Re: [kicad-users] Mixed part types with multi-part components?


?
It can be done fairly easily.
I created a relay symbol that had the coil and contacts as sep parts.

In the component properties you need to set the number of parts, I expect
that you have done this for other parts you have created.

Then you can start editing the component. In the top toolbar there are
two boxes, one to select the part A, B, C and so on. then a box for the
name. Next to that box is a button "edit pins per part or body style"

Click this so that it is active. this setting allows you to use
different designs and pins for each sub part.

If I remember correctly there was a small problem in getting things to
edit correctly, and what I did was to just put a single line on all
parts (with the edit pins button unselected, then switch it back on and
I could then edit things as normal.  I've not tried to do this with my
current version of kicad,  BZR 3256, so that little problem may have
been sorted out by now.

Andy

On Thu, 12 Apr 2012 22:33:21 -0000
"acousmatique" <acousmatique@...> wrote:

Arg... this is driving me nuts.

For the past two weeks, I have buckled down to create the partslibraries I need. This seems to be a nightmare for every program I try, like
they assume the parts you need are already there.

I have made some multi-part profiles which have turned out well. Theproblem seems to be when I am making a component which has multiple parts, but
they aren't all the same. For instance, tonight I am trying to make a big
library of transistor and diode arrays that I use. Now I am trying to enter a
device (THAT 340) which has two NPN transistors, and two PNP transistors. I
define pins 1-3 as NPN for Part A, but then when I define pins 5-7 as PNP for
Part B, I go back and it has overwritten the PNP for PART A also! I cannot
imagine any reason why this would happen. They have their own pin numbers! If
I change the part for pins 5-7 why would it assume that I am changing pins 1-3
which I have already done?

The only workaround I can think of for now is just using a monolithicblock and naming the pins for the whole device. It's easy, but it makes the
schematics messy. Any ideas? Am I missing something here?

Thanks!



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

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

rohchar

#12222

Hi,

see below :

regards,
Charles.

Show quoted text

--- In kicad-users@..., "rertelt" <rertelt@...> wrote:

For the pins it work well, but with the artwork KiCAD had some problem:

On all parts it places the same artwork. I call it a bug...

Roland

--- In kicad-users@..., Ivica Kvasina <kvasina@> wrote:

creating different artwork for each part is a problem.??
every time i change one part, change is applied to all of them.
i did try various settings incl. edit pins per part but so far this is still frustrating.

开云体育

Mixed part types with multi-part components?