Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-23 Thread Robert
 The error occurs only when I try to create a PCB without schematic
 nor netlist AND with the DRC active. I don't get any error when the
 DRC is OFF, or if I have a schematic and a proper netlist.

That's because you can't have DRC without a netlist; please see my last 
post on this subject for the explanation.

Regards,

Robert.
No virus found in this outgoing message.
Checked by AVG - www.avg.com 
Version: 9.0.851 / Virus Database: 271.1.1/3088 - Release Date: 08/22/10 
19:35:00


Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread Robert
 Well, I am human! Therefore, when something try to NOT LET ME do
 things, I tend to struggle :) It works when I turn the DRC off, but
 it looks messy, and then I loose the isolation check and the comfort
 of the isolation zones delimited. That's why I would like to keep the
 DRC on...

You can't have DRC without a netlist, because the netlist is what tells 
PCBNew what can and can't be connected.   You can create a netlist 
manually (it's a text file), but the quickest, easiest, most reliable 
way to generate a netlist is with a schematic editor.   I create a 
schematic even for very simple boards because it allows me to leave DRC 
on, ensuring my board is neat and correct first time.   If the schematic 
is purely being used as a means of generating a netlist and I don't have 
the exact component in the library, I save time by improvising with 
something similar (because PCBNew only cares about footprints and 
connectivity, not electrical properties).

I used to use ISIS, and churned out one scrap board after another. 
Since using Kicad (with DRC on) that no longer happens.   Kicad is a far 
better tool for producing boards, but only if you don't force it to 
behave like obsolete software.

Regards,

Robert.


 I don't see how I could make a netlist without drawing a schematic
 first?

 Axel


 --- In kicad-users@yahoogroups.com, Cat Ccatalin_c...@...  wrote:


 Did you turn DRC off?

 That's the purpose of DRC, to NOT LET YOU do things that are not in
 the netlist (among other things).

 If you don't want to make a schematic, make a netlist.



 Cat

 To: kicad-users@yahoogroups.com From: mad...@... Date: Fri, 20
 Aug 2010 23:40:39 + Subject: [kicad-users] Re: Type Err(4)
 trace near pad issue in Kicad

 Well, I made a simple schematic with EEschema, passed the
 electrical check without trouble, made the netlist, did the CVpcb
 thing, and routed in PCBnew. All is fine, so my Kicad build seems
 to be working.

 I tried to add another module in the pcb. Fine. I tried to
 connect the new module with a trace... Type Err(4)! It doesn't
 agree to connect the trace to the new component.

 I still don't understand why I cannot route manually without a
 schematic or a netlist when the faq says I could?

 Axel





 

 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 http://www.kicadlib.org 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
 http://groups.yahoo.com/group/kicad-develYahoo! Groups Links





 No virus found in this incoming message. Checked by AVG -
 www.avg.com Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release
 Date: 08/20/10 07:35:00

No virus found in this outgoing message.
Checked by AVG - www.avg.com 
Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release Date: 08/20/10 
07:35:00


[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread ma...@ymail.com
I understand the idea of following a logical path schemanetlistpcb... It's a 
better way, it's safer, it's perfect for learning, and so on. And when I'm 
designing, that's how I want to work. But for some applications it's plain 
frustrating, if not time wasting! Let me give you an example:

Part of my job is maintenance for vintage audio equipment. Say an old console 
comes in and needs 4 more channel strips. Those are 'unobtainable', 
manufacturer has closed years ago, spare parts and schematics are unavailable, 
but the thing is old enough so there's no copyright or patent issue. So my job 
is to make some new PCBs and populate them. We are talking a big pcb, with 300+ 
components. Some of them are obsolete, so I really need to redraw the PCB to 
accommodate newer parts. 
Using good photographs of the original board, and transparent windows, I can 
redraw the whole thing in about a day... Job done.
Now if I have to trace out the schemo, we are talking at least two more days of 
work!

Maybe I just need to use obsolete tools to work with vintage stuff :)

For this kind of job, the latest brand new and up-to-date software would be the 
one who allows me to draw the pcb first, THEN generate a netlist from the pcb, 
and then read this netlist IN the schematic editor so I could arrange them in a 
readable order...

Bah, guess I should stop dreaming about simple things that could make life 
simpler...

Axel

--- In kicad-users@yahoogroups.com, Robert birmingham_spi...@... wrote:

  Well, I am human! Therefore, when something try to NOT LET ME do
  things, I tend to struggle :) It works when I turn the DRC off, but
  it looks messy, and then I loose the isolation check and the comfort
  of the isolation zones delimited. That's why I would like to keep the
  DRC on...
 
 You can't have DRC without a netlist, because the netlist is what tells 
 PCBNew what can and can't be connected.   You can create a netlist 
 manually (it's a text file), but the quickest, easiest, most reliable 
 way to generate a netlist is with a schematic editor.   I create a 
 schematic even for very simple boards because it allows me to leave DRC 
 on, ensuring my board is neat and correct first time.   If the schematic 
 is purely being used as a means of generating a netlist and I don't have 
 the exact component in the library, I save time by improvising with 
 something similar (because PCBNew only cares about footprints and 
 connectivity, not electrical properties).
 
 I used to use ISIS, and churned out one scrap board after another. 
 Since using Kicad (with DRC on) that no longer happens.   Kicad is a far 
 better tool for producing boards, but only if you don't force it to 
 behave like obsolete software.
 
 Regards,
 
 Robert.
 
 
  I don't see how I could make a netlist without drawing a schematic
  first?
 
  Axel
 
 
  --- In kicad-users@yahoogroups.com, Cat Ccatalin_cluj@  wrote:
 
 
  Did you turn DRC off?
 
  That's the purpose of DRC, to NOT LET YOU do things that are not in
  the netlist (among other things).
 
  If you don't want to make a schematic, make a netlist.
 
 
 
  Cat
 
  To: kicad-users@yahoogroups.com From: mad.ax@ Date: Fri, 20
  Aug 2010 23:40:39 + Subject: [kicad-users] Re: Type Err(4)
  trace near pad issue in Kicad
 
  Well, I made a simple schematic with EEschema, passed the
  electrical check without trouble, made the netlist, did the CVpcb
  thing, and routed in PCBnew. All is fine, so my Kicad build seems
  to be working.
 
  I tried to add another module in the pcb. Fine. I tried to
  connect the new module with a trace... Type Err(4)! It doesn't
  agree to connect the trace to the new component.
 
  I still don't understand why I cannot route manually without a
  schematic or a netlist when the faq says I could?
 
  Axel
 
 
 
 
 
  
 
  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 http://www.kicadlib.org 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
  http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
 
 
 
 
 
  No virus found in this incoming message. Checked by AVG -
  www.avg.com Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release
  Date: 08/20/10 07:35:00
 
 
 
 No virus found in this outgoing message.
 Checked by AVG - www.avg.com 
 Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release Date: 08/20/10 
 07:35:00





Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread Andy Eskelson
Odd - not much I can add at this point. If you want, you can upload
your files (best to put the sch, brd and netlist or as many of them as
you have) to the files section and I'll have a look at it. (or email them
to me directly)

There maybe some other infringement of the rules going on that you have
not spotted as yet.


You CAN create PCB's manually. You have to turn off all the DRC rules.
However you then miss out on the protection that DRC gives you.

preferences  general (middle of the window, DRC on/off tickbox)
I'm still using the 2009 linux version of Kicad, so in the latest verson
the menu locations may have changed.

When you use DRC and then add a module, the system will complain, as DRC
will not know anything about this component. 


Andy


On Fri, 20 Aug 2010 22:34:07 -
ma...@ymail.com mad...@free.fr wrote:

 Thank you for your answer. Maybe I'm thinking too simple, or Old school... 
 Last time I successfully used a CAD was 15 years ago. Back then I could 
 certainly make a PCB with Proteus lite without using ISIS (the schematic 
 editor) nor making a netlist... According to the Kicad FAQ, I should be able 
 to work this way...
 5.1 How do I manually route a PCB?
 Manual routing is quite straight forward. You don't even need to have a 
 schematic.
 
 I tried the thinnest trace possible, and even straight (with no angle at all) 
 the error occurs!
 
 Axel
 
 --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote:
 
  The problem is that you are thinking too simple...
  
  KIcad like most design software is designed to work via netlists and so
  on.
  
  As has been suggested you could simply turn off the design rules checking
  that will prevent errors and so on.
  
  By far the best method is to create a simple sch. in eeschema and then
  use that to generate the required netlist. 
  
  It's well worth getting used to creating the circuit then the PCB and so
  on.
  
  The error is just giving you a warning that a track is too close to a pad.
  
  Tracks and pads have a clearance setting. The normal problkem is that you
  cut across the pad at an angle with a track, and you just clip the edge
  of the clearance limit. Centre on where the error is and zoom right in,
  and you will prob see the problem.
  
  Use a slightly thinner track, or re-route it to miss the clearance area.
  
  Like most packages Kicad takes a bit of getting used to, I used a lot
  worse! (and not just PCB packages)
  
  Andy
   
  
  
  
  On Fri, 20 Aug 2010 08:39:38 -
  ma...@... mad...@... wrote:
  
   Hello group!
   This is my first post, so I apologize but I'm afraid I need some help!
   
   I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far 
   as drawing schematics, everything is ok. Now if I try to draw a PCB 
   without schematic, without netlist, without autorouter... Just a simple 
   one sided circuit board. I create a new project, open PCB new, place say 
   a DIP-8_300 component, click on 'add traces and vias', start tracing... 
   and get:
   Type Err(4) trace near pad
   
   What the hell am I doing wrong?
   I can draw a trace without problem as long as I don't get near to the 
   component (which is not very useful!). It's not component related (same 
   behavior with resistances, caps, and so on)
   Component and traces are both on the 'under' side. I tried different 
   traces sizes, I searched in the manual, in the different tutos, in the 
   web... Nada! I searched here but the search server is 'busy' please try 
   again later! Plus I don't know what to enter in the search engine, 
   'manual routing' return results such as auto-routing in the kicad manual, 
   and the likes!
   
   I'm quite convinced that this must be something really simple, but I 
   can't find it!
   
   Thanks for your help
   Axel
   
   
   
   
   
   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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! 
   Groups Links
   
   
  
 
 
 
 
 
 
 
 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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
 Links
 
 
 


[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread ma...@ymail.com
The error occurs only when I try to create a PCB without schematic nor netlist 
AND with the DRC active. I don't get any error when the DRC is OFF, or if I 
have a schematic and a proper netlist.

So I guess my problem was that I expected PCBnew to work as a standalone app 
WITH DRC. Obviously it is not the case. Either I respect the workflow 
(schematicnetlistCVpcbPCBnew) which I understand and agree to when in 
'designer' mode, either I have to sacrifice the DRC safety when I want to save 
some time and draw a PCB from scratch.

Thanks to all for helping me clarifying that out!

Axel


--- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote:

 Odd - not much I can add at this point. If you want, you can upload
 your files (best to put the sch, brd and netlist or as many of them as
 you have) to the files section and I'll have a look at it. (or email them
 to me directly)
 
 There maybe some other infringement of the rules going on that you have
 not spotted as yet.
 
 
 You CAN create PCB's manually. You have to turn off all the DRC rules.
 However you then miss out on the protection that DRC gives you.
 
 preferences  general (middle of the window, DRC on/off tickbox)
 I'm still using the 2009 linux version of Kicad, so in the latest verson
 the menu locations may have changed.
 
 When you use DRC and then add a module, the system will complain, as DRC
 will not know anything about this component. 
 
 
 Andy
 
 
 On Fri, 20 Aug 2010 22:34:07 -
 ma...@... mad...@... wrote:
 
  Thank you for your answer. Maybe I'm thinking too simple, or Old school... 
  Last time I successfully used a CAD was 15 years ago. Back then I could 
  certainly make a PCB with Proteus lite without using ISIS (the schematic 
  editor) nor making a netlist... According to the Kicad FAQ, I should be 
  able to work this way...
  5.1 How do I manually route a PCB?
  Manual routing is quite straight forward. You don't even need to have a 
  schematic.
  
  I tried the thinnest trace possible, and even straight (with no angle at 
  all) the error occurs!
  
  Axel
  
  --- In kicad-users@yahoogroups.com, Andy Eskelson andyyahoo@ wrote:
  
   The problem is that you are thinking too simple...
   
   KIcad like most design software is designed to work via netlists and so
   on.
   
   As has been suggested you could simply turn off the design rules checking
   that will prevent errors and so on.
   
   By far the best method is to create a simple sch. in eeschema and then
   use that to generate the required netlist. 
   
   It's well worth getting used to creating the circuit then the PCB and so
   on.
   
   The error is just giving you a warning that a track is too close to a pad.
   
   Tracks and pads have a clearance setting. The normal problkem is that you
   cut across the pad at an angle with a track, and you just clip the edge
   of the clearance limit. Centre on where the error is and zoom right in,
   and you will prob see the problem.
   
   Use a slightly thinner track, or re-route it to miss the clearance area.
   
   Like most packages Kicad takes a bit of getting used to, I used a lot
   worse! (and not just PCB packages)
   
   Andy

   
   
   
   On Fri, 20 Aug 2010 08:39:38 -
   madax@ mad.ax@ wrote:
   
Hello group!
This is my first post, so I apologize but I'm afraid I need some help!

I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far 
as drawing schematics, everything is ok. Now if I try to draw a PCB 
without schematic, without netlist, without autorouter... Just a simple 
one sided circuit board. I create a new project, open PCB new, place 
say a DIP-8_300 component, click on 'add traces and vias', start 
tracing... and get:
Type Err(4) trace near pad

What the hell am I doing wrong?
I can draw a trace without problem as long as I don't get near to the 
component (which is not very useful!). It's not component related (same 
behavior with resistances, caps, and so on)
Component and traces are both on the 'under' side. I tried different 
traces sizes, I searched in the manual, in the different tutos, in the 
web... Nada! I searched here but the search server is 'busy' please try 
again later! Plus I don't know what to enter in the search engine, 
'manual routing' return results such as auto-routing in the kicad 
manual, and the likes!

I'm quite convinced that this must be something really simple, but I 
can't find it!

Thanks for your help
Axel





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 http://www.kicadlib.org for details of how to contribute 
your symbols/modules to the kicad library.
For building Kicad from source and other 

Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread Andy Eskelson

Yes, you are correct, DRC NEEDs other info in order to work.

In regards to your old PCB requirement, many years ago when we had a
similar situation in needing to recreate a PCB when the tape masters had
been lost we would put the PCB on the copy camera and take a pic of it.
If the board was rather dense, we would sometimes tweak the enlargement
factor slightly to get the sizes 100% correct. Using the hi contrast
films, we usually got an acceptable image for reproducing the PCB. A
little lightbox work was sometimes needed but not often.

You could prob. do just as well if not a better job  with a good quality
flatbed scanner. 

Andy





On Sat, 21 Aug 2010 11:53:13 -
ma...@ymail.com mad...@free.fr wrote:

 The error occurs only when I try to create a PCB without schematic nor 
 netlist AND with the DRC active. I don't get any error when the DRC is OFF, 
 or if I have a schematic and a proper netlist.
 
 So I guess my problem was that I expected PCBnew to work as a standalone app 
 WITH DRC. Obviously it is not the case. Either I respect the workflow 
 (schematicnetlistCVpcbPCBnew) which I understand and agree to when in 
 'designer' mode, either I have to sacrifice the DRC safety when I want to 
 save some time and draw a PCB from scratch.
 
 Thanks to all for helping me clarifying that out!
 
 Axel
 
 
 --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote:
 
  Odd - not much I can add at this point. If you want, you can upload
  your files (best to put the sch, brd and netlist or as many of them as
  you have) to the files section and I'll have a look at it. (or email them
  to me directly)
  
  There maybe some other infringement of the rules going on that you have
  not spotted as yet.
  
  
  You CAN create PCB's manually. You have to turn off all the DRC rules.
  However you then miss out on the protection that DRC gives you.
  
  preferences  general (middle of the window, DRC on/off tickbox)
  I'm still using the 2009 linux version of Kicad, so in the latest verson
  the menu locations may have changed.
  
  When you use DRC and then add a module, the system will complain, as DRC
  will not know anything about this component. 
  
  
  Andy
  
  
  On Fri, 20 Aug 2010 22:34:07 -
  ma...@... mad...@... wrote:
  
   Thank you for your answer. Maybe I'm thinking too simple, or Old 
   school... Last time I successfully used a CAD was 15 years ago. Back then 
   I could certainly make a PCB with Proteus lite without using ISIS (the 
   schematic editor) nor making a netlist... According to the Kicad FAQ, I 
   should be able to work this way...
   5.1 How do I manually route a PCB?
   Manual routing is quite straight forward. You don't even need to have a 
   schematic.
   
   I tried the thinnest trace possible, and even straight (with no angle at 
   all) the error occurs!
   
   Axel
   
   --- In kicad-users@yahoogroups.com, Andy Eskelson andyyahoo@ wrote:
   
The problem is that you are thinking too simple...

KIcad like most design software is designed to work via netlists and so
on.

As has been suggested you could simply turn off the design rules 
checking
that will prevent errors and so on.

By far the best method is to create a simple sch. in eeschema and then
use that to generate the required netlist. 

It's well worth getting used to creating the circuit then the PCB and so
on.

The error is just giving you a warning that a track is too close to a 
pad.

Tracks and pads have a clearance setting. The normal problkem is that 
you
cut across the pad at an angle with a track, and you just clip the edge
of the clearance limit. Centre on where the error is and zoom right in,
and you will prob see the problem.

Use a slightly thinner track, or re-route it to miss the clearance area.

Like most packages Kicad takes a bit of getting used to, I used a lot
worse! (and not just PCB packages)

Andy
 



On Fri, 20 Aug 2010 08:39:38 -
madax@ mad.ax@ wrote:

 Hello group!
 This is my first post, so I apologize but I'm afraid I need some help!
 
 I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As 
 far as drawing schematics, everything is ok. Now if I try to draw a 
 PCB without schematic, without netlist, without autorouter... Just a 
 simple one sided circuit board. I create a new project, open PCB new, 
 place say a DIP-8_300 component, click on 'add traces and vias', 
 start tracing... and get:
 Type Err(4) trace near pad
 
 What the hell am I doing wrong?
 I can draw a trace without problem as long as I don't get near to the 
 component (which is not very useful!). It's not component related 
 (same behavior with resistances, caps, and so on)
 Component and traces are both on the 'under' side. I tried different 
 traces sizes, I searched in 

[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-21 Thread ma...@ymail.com
I remember doing the poor man's version of this kind of job with a xerox 
machine, a pair of scissor, and a black waterproof marker!
That was before I could afford a scanner!
I know a guy who etches hundreds of PCB each month, and he uses nothing but 
Illustrator.
But being an electronic tech, I'd rather spend nights learning Kicad than 
Inkscape. And the ability to replace an obsolete package by a new one with a 
simple click is indeed a feature I use often, especially when dealing with 
20yo+ stuff...


Axel

--- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote:

 
 Yes, you are correct, DRC NEEDs other info in order to work.
 
 In regards to your old PCB requirement, many years ago when we had a
 similar situation in needing to recreate a PCB when the tape masters had
 been lost we would put the PCB on the copy camera and take a pic of it.
 If the board was rather dense, we would sometimes tweak the enlargement
 factor slightly to get the sizes 100% correct. Using the hi contrast
 films, we usually got an acceptable image for reproducing the PCB. A
 little lightbox work was sometimes needed but not often.
 
 You could prob. do just as well if not a better job  with a good quality
 flatbed scanner. 
 
 Andy
 
 
 
 
 
 On Sat, 21 Aug 2010 11:53:13 -
 ma...@... mad...@... wrote:
 
  The error occurs only when I try to create a PCB without schematic nor 
  netlist AND with the DRC active. I don't get any error when the DRC is OFF, 
  or if I have a schematic and a proper netlist.
  
  So I guess my problem was that I expected PCBnew to work as a standalone 
  app WITH DRC. Obviously it is not the case. Either I respect the workflow 
  (schematicnetlistCVpcbPCBnew) which I understand and agree to when in 
  'designer' mode, either I have to sacrifice the DRC safety when I want to 
  save some time and draw a PCB from scratch.
  
  Thanks to all for helping me clarifying that out!
  
  Axel
  
  
  --- In kicad-users@yahoogroups.com, Andy Eskelson andyyahoo@ wrote:
  
   Odd - not much I can add at this point. If you want, you can upload
   your files (best to put the sch, brd and netlist or as many of them as
   you have) to the files section and I'll have a look at it. (or email them
   to me directly)
   
   There maybe some other infringement of the rules going on that you have
   not spotted as yet.
   
   
   You CAN create PCB's manually. You have to turn off all the DRC rules.
   However you then miss out on the protection that DRC gives you.
   
   preferences  general (middle of the window, DRC on/off tickbox)
   I'm still using the 2009 linux version of Kicad, so in the latest verson
   the menu locations may have changed.
   
   When you use DRC and then add a module, the system will complain, as DRC
   will not know anything about this component. 
   
   
   Andy
   
   
   On Fri, 20 Aug 2010 22:34:07 -
   madax@ mad.ax@ wrote:
   
Thank you for your answer. Maybe I'm thinking too simple, or Old 
school... Last time I successfully used a CAD was 15 years ago. Back 
then I could certainly make a PCB with Proteus lite without using ISIS 
(the schematic editor) nor making a netlist... According to the Kicad 
FAQ, I should be able to work this way...
5.1 How do I manually route a PCB?
Manual routing is quite straight forward. You don't even need to have a 
schematic.

I tried the thinnest trace possible, and even straight (with no angle 
at all) the error occurs!

Axel

--- In kicad-users@yahoogroups.com, Andy Eskelson andyyahoo@ wrote:

 The problem is that you are thinking too simple...
 
 KIcad like most design software is designed to work via netlists and 
 so
 on.
 
 As has been suggested you could simply turn off the design rules 
 checking
 that will prevent errors and so on.
 
 By far the best method is to create a simple sch. in eeschema and then
 use that to generate the required netlist. 
 
 It's well worth getting used to creating the circuit then the PCB and 
 so
 on.
 
 The error is just giving you a warning that a track is too close to a 
 pad.
 
 Tracks and pads have a clearance setting. The normal problkem is that 
 you
 cut across the pad at an angle with a track, and you just clip the 
 edge
 of the clearance limit. Centre on where the error is and zoom right 
 in,
 and you will prob see the problem.
 
 Use a slightly thinner track, or re-route it to miss the clearance 
 area.
 
 Like most packages Kicad takes a bit of getting used to, I used a lot
 worse! (and not just PCB packages)
 
 Andy
  
 
 
 
 On Fri, 20 Aug 2010 08:39:38 -
 madax@ mad.ax@ wrote:
 
  Hello group!
  This is my first post, so I apologize but I'm afraid I need some 
  help!
  
  I installed Kicad (2010-05-05 BZR 2356) on Ubuntu 

[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-20 Thread ma...@ymail.com
Thank you for your answers. I certainly agree that disabling the DRC is not a 
good thing. If I should not need the DRC, I could as well use the Gimp to make 
my PCB! It would certainly give me a better output on my laser printer :)
I can think of a few cases when creating a schematic would not be easier nor 
quickier...  And according to the Kicad FAQ, chapter 5.1:
5.1 How do I manually route a PCB?
Manual routing is quite straight forward. You don't even need to have a 
schematic.

That's exactly what I would like to do...

Axel

--- In kicad-users@yahoogroups.com, Robert birmingham_spi...@... wrote:

 The OP is certainly going to need good luck if he turns off the DRC. 
 Turning it off may well allow the track to be placed, but since the DRC 
 is there to dramatically reduce the chances of designing a scrap board, 
 in the long run it is quicker and easier to create a schematic and leave 
 the DRC on, even for a simple board (and just think how many ways 
 there are of misconnecting a rectangular box with eight legs).   Not 
 doing so is like being given a ruler to help you draw a straight line, 
 but not using it in order to save the time involved in placing it on the 
 the paper.
 
 Regards,
 
 Robert.
 
 On 20/08/2010 15:18, Cat C wrote:
 
  I think you need to turn DRC (Design Rules Checking) off, but I'm a 
  beginner too, so I'm not sure.
 
 
 
  Good luck,
 
 
 
  Cat
 
 
  To: kicad-users@yahoogroups.com
  From: mad...@...
  ...
 
  I create a new project, open PCB new, place say a DIP-8_300 component, 
  click on 'add traces and vias', start tracing... and get:
  Type Err(4) trace near pad
 
  ...
  
 
 
 
 
  No virus found in this incoming message.
  Checked by AVG - www.avg.com
  Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release Date: 08/20/10 
  07:35:00
 
 
 
 No virus found in this outgoing message.
 Checked by AVG - www.avg.com 
 Version: 9.0.851 / Virus Database: 271.1.1/3083 - Release Date: 08/20/10 
 07:35:00





[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-20 Thread ma...@ymail.com
Thank you for your answer. I will try to make a simple schematic and netlist, 
to see if it works better... But it is my understanding that I shouldn't be 
forced to go through those steps.

Axel

--- In kicad-users@yahoogroups.com, Ricardo Cárdenes Medina 
ricardo.carde...@... wrote:

 On Fri, Aug 20, 2010 at 9:39 AM, ma...@... mad...@... wrote:
 
 
 
  Hello group!
  This is my first post, so I apologize but I'm afraid I need some help!
 
  I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far as
  drawing schematics, everything is ok. Now if I try to draw a PCB without
  schematic, without netlist, without autorouter... Just a simple one sided
  circuit board. I create a new project, open PCB new, place say a DIP-8_300
  component, click on 'add traces and vias', start tracing... and get:
  Type Err(4) trace near pad
 
  What the hell am I doing wrong.
 
 As far as I can see, the problem is that you're trying to draw a track
 to/from a pad that doesn't have a net assigned. How to assign a net to a
 pad? Editing the pad of course, but as you're coming from a blank
 situation, with no netlist, then I don't know how it works... Tagging a pad
 with a net that doesn't exists will actually crash my pcbnew.





[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-20 Thread ma...@ymail.com
Thank you for your answer. Maybe I'm thinking too simple, or Old school... Last 
time I successfully used a CAD was 15 years ago. Back then I could certainly 
make a PCB with Proteus lite without using ISIS (the schematic editor) nor 
making a netlist... According to the Kicad FAQ, I should be able to work this 
way...
5.1 How do I manually route a PCB?
Manual routing is quite straight forward. You don't even need to have a 
schematic.

I tried the thinnest trace possible, and even straight (with no angle at all) 
the error occurs!

Axel

--- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote:

 The problem is that you are thinking too simple...
 
 KIcad like most design software is designed to work via netlists and so
 on.
 
 As has been suggested you could simply turn off the design rules checking
 that will prevent errors and so on.
 
 By far the best method is to create a simple sch. in eeschema and then
 use that to generate the required netlist. 
 
 It's well worth getting used to creating the circuit then the PCB and so
 on.
 
 The error is just giving you a warning that a track is too close to a pad.
 
 Tracks and pads have a clearance setting. The normal problkem is that you
 cut across the pad at an angle with a track, and you just clip the edge
 of the clearance limit. Centre on where the error is and zoom right in,
 and you will prob see the problem.
 
 Use a slightly thinner track, or re-route it to miss the clearance area.
 
 Like most packages Kicad takes a bit of getting used to, I used a lot
 worse! (and not just PCB packages)
 
 Andy
  
 
 
 
 On Fri, 20 Aug 2010 08:39:38 -
 ma...@... mad...@... wrote:
 
  Hello group!
  This is my first post, so I apologize but I'm afraid I need some help!
  
  I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far as 
  drawing schematics, everything is ok. Now if I try to draw a PCB without 
  schematic, without netlist, without autorouter... Just a simple one sided 
  circuit board. I create a new project, open PCB new, place say a DIP-8_300 
  component, click on 'add traces and vias', start tracing... and get:
  Type Err(4) trace near pad
  
  What the hell am I doing wrong?
  I can draw a trace without problem as long as I don't get near to the 
  component (which is not very useful!). It's not component related (same 
  behavior with resistances, caps, and so on)
  Component and traces are both on the 'under' side. I tried different traces 
  sizes, I searched in the manual, in the different tutos, in the web... 
  Nada! I searched here but the search server is 'busy' please try again 
  later! Plus I don't know what to enter in the search engine, 'manual 
  routing' return results such as auto-routing in the kicad manual, and the 
  likes!
  
  I'm quite convinced that this must be something really simple, but I can't 
  find it!
  
  Thanks for your help
  Axel
  
  
  
  
  
  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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
  Links
  
  
 





[kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-20 Thread ma...@ymail.com
Well, I made a simple schematic with EEschema, passed the electrical check 
without trouble, made the netlist, did the CVpcb thing, and routed in PCBnew. 
All is fine, so my Kicad build seems to be working.

I tried to add another module in the pcb. Fine.
I tried to connect the new module with a trace... Type Err(4)!
It doesn't agree to connect the trace to the new component. 

I still don't understand why I cannot route manually without a schematic or a 
netlist when the faq says I could?

Axel

--- In kicad-users@yahoogroups.com, ma...@... mad...@... wrote:

 Thank you for your answer. I will try to make a simple schematic and netlist, 
 to see if it works better... But it is my understanding that I shouldn't be 
 forced to go through those steps.
 
 Axel
 
 --- In kicad-users@yahoogroups.com, Ricardo Cárdenes Medina 
 ricardo.cardenes@ wrote:
 
  On Fri, Aug 20, 2010 at 9:39 AM, madax@ mad.ax@ wrote:
  
  
  
   Hello group!
   This is my first post, so I apologize but I'm afraid I need some help!
  
   I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far as
   drawing schematics, everything is ok. Now if I try to draw a PCB without
   schematic, without netlist, without autorouter... Just a simple one sided
   circuit board. I create a new project, open PCB new, place say a DIP-8_300
   component, click on 'add traces and vias', start tracing... and get:
   Type Err(4) trace near pad
  
   What the hell am I doing wrong.
  
  As far as I can see, the problem is that you're trying to draw a track
  to/from a pad that doesn't have a net assigned. How to assign a net to a
  pad? Editing the pad of course, but as you're coming from a blank
  situation, with no netlist, then I don't know how it works... Tagging a pad
  with a net that doesn't exists will actually crash my pcbnew.
 





RE: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad

2010-08-20 Thread Cat C

Did you turn DRC off?

That's the purpose of DRC, to NOT LET YOU do things that are not in the netlist 
(among other things).

If you don't want to make a schematic, make a netlist.

 

Cat
 
 To: kicad-users@yahoogroups.com
 From: mad...@free.fr
 Date: Fri, 20 Aug 2010 23:40:39 +
 Subject: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad
 
 Well, I made a simple schematic with EEschema, passed the electrical check 
 without trouble, made the netlist, did the CVpcb thing, and routed in PCBnew. 
 All is fine, so my Kicad build seems to be working.
 
 I tried to add another module in the pcb. Fine.
 I tried to connect the new module with a trace... Type Err(4)!
 It doesn't agree to connect the trace to the new component. 
 
 I still don't understand why I cannot route manually without a schematic or a 
 netlist when the faq says I could?
 
 Axel