pcb

Vias tented

Bug #1744832 reported by Dr M on 2018-01-23
12
This bug affects 2 people
Affects Status Importance Assigned to Milestone
pcb
Medium
Chad Parker

Bug Description

Vias are created tented. So far, I have not found any description in the manual of to how to change this behavior, nor any description of how to un-tent the via once it has been created. I did see a mention in a blog that there is keyboard shortcut, "k", this does not seem to work. I have been correcting this manually by editing the PCB file.

Bert Timmerman (bert-timmerman) wrote :

Hi,

I tried to reproduce this bug with pcb-4.0.2 (in the gtk UI).

The command MinMaskGap executed within the pcb command entry (invoked with ":") works as advertised in the manual for pins in elements.

For example ":MinMaskGap(Selected,1.0mm)" gives the result on a single selected pin inside an elemnet.

This does not work for me on a single selected via (either solo or inside a polygon, with or without thermals).

So I can confirm this bug for pcb-4.0.2.

Kind regards,

Bert Timmerman.

Changed in pcb:
status: New → Confirmed
Changed in pcb:
importance: Undecided → Medium
Changed in pcb:
milestone: none → pcb-4.1.1
Bert Timmerman (bert-timmerman) wrote :

Hi,

This bug is getting strange ...

Searching the web I found a 9 year old mailing list thread you mentioned in your initial report (http://geda-user.delorie.narkive.com/6GluA3z7/deafult-gap-between-copper-pin-pad-and-resist).

This thread mentions hovering over the tented via and pressing [k] or [shift]+[k] for increasing/decreasing the gap ... this works for me as expected.

Invoking the "MinMaskGap(Selected,1.5mm)" command in the command entry worked too after this test, except in one instance ... and after that it resumed working.

Bug report #929123 mentions fragile code ... and it looks like that indeed.

I think this issue needs to be addressed after the pcb-4.1.0 release so I put these two reports on the pcb-4.1.1 todo list.

To be continued.

Kind regards,

Bert Timmerman.

The "k" does not work for me.

I think I might differ in the severity. This would be a real show stopper
except for manually editing the PCB file.

On Jan 24, 2018 7:30 PM, "Bert Timmerman" <email address hidden>
wrote:

> Hi,
>
> This bug is getting strange ...
>
> Searching the web I found a 9 year old mailing list thread you mentioned
> in your initial report (http://geda-user.delorie.narkive.com/6GluA3z7
> /deafult-gap-between-copper-pin-pad-and-resist).
>
> This thread mentions hovering over the tented via and pressing [k] or
> [shift]+[k] for increasing/decreasing the gap ... this works for me as
> expected.
>
> Invoking the "MinMaskGap(Selected,1.5mm)" command in the command entry
> worked too after this test, except in one instance ... and after that it
> resumed working.
>
> Bug report #929123 mentions fragile code ... and it looks like that
> indeed.
>
> I think this issue needs to be addressed after the pcb-4.1.0 release so
> I put these two reports on the pcb-4.1.1 todo list.
>
> To be continued.
>
> Kind regards,
>
> Bert Timmerman.
>
> --
> You received this bug notification because you are subscribed to the bug
> report.
> https://bugs.launchpad.net/bugs/1744832
>
> Title:
> Vias tented
>
> Status in pcb:
> Confirmed
>
> Bug description:
> Vias are created tented. So far, I have not found any description in
> the manual of to how to change this behavior, nor any description of
> how to un-tent the via once it has been created. I did see a mention
> in a blog that there is keyboard shortcut, "k", this does not seem to
> work. I have been correcting this manually by editing the PCB file.
>
> To manage notifications about this bug go to:
> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>

Chad Parker (parker-charles) wrote :

Dr M- What version of pcb are you using?

I'm concerned that the "k" command isn't working for you. It seems to work for Bert, and it works for me also. You may have to press it several times for the opening to be large enough.

Bert- I'm not able to get MinMaskGap(Selected, 1.5mm) to operate on the vias. I only see it operate on pins.

Dr M (drmcn) wrote :

The following is from the "help - about" item,

    This is PCB, an interactive
    printed circuit board editor
    version 20140316

    Compiled on Feb 11 2017 at 11:18:48

    by harry eaton

On 03/04/2018 10:47 AM, Chad Parker wrote:
> Dr M- What version of pcb are you using?
>
> I'm concerned that the "k" command isn't working for you. It seems to
> work for Bert, and it works for me also. You may have to press it
> several times for the opening to be large enough.
>
> Bert- I'm not able to get MinMaskGap(Selected, 1.5mm) to operate on the
> vias. I only see it operate on pins.
>

Chad Parker (parker-charles) wrote :

Dr. M-

Sorry for the delay... the last couple weeks have been rough at work.

The version of pcb you're using is quite old. Are you able to upgrade to the latest 4.1 series?

I think the real solution to this is to add solder mask clearance to the route styles.

Chad Parker (parker-charles) wrote :

Dr. M-

I've pushed a branch to the git repository: home/cparker/route_styles_via_sm_clearance

In this branch, the solder mask aperture can be configured using the route styles interface. You'll have to update existing vias by hand, but you should be able to create new vias with clearance you specify.

Please test if you are able.

Bert-

This branch includes a change to the file format, to add the via mask clearance to the styles string. If the clearance are all zero (default), then it uses the old format so as to be backwards compatible.

I haven't been able to test the lesstif hid yet... they updated something on my Mac and now Motif is seg faulting...

Cheers,
--Chad

Changed in pcb:
status: Confirmed → In Progress
Dr M (drmcn) wrote :

Hi Bert

Thank you for that.  Hopefully, the file format is backward compatible.
   I have a lot of python code invested in generating boards with large
arrays of sensors and amplifiers.

I have been working with the version that is provided by Fedora and
included in their collection of electronics CAD software. That they use
a version that it so wildly out of date, suggests that one of the
problems is that Fedora does not have somebody to maintain this properly
in their repositories.

So, I have to study the issue a little bit to determine how to bring in
the current version without causing a code maintenance burden with
subsequent system updates and upgrades.

Regards

Dr Mitch

On 03/18/2018 06:25 PM, Chad Parker wrote:
> Dr. M-
>
> I've pushed a branch to the git repository:
> home/cparker/route_styles_via_sm_clearance
>
> In this branch, the solder mask aperture can be configured using the
> route styles interface. You'll have to update existing vias by hand, but
> you should be able to create new vias with clearance you specify.
>
> Please test if you are able.
>
> Bert-
>
> This branch includes a change to the file format, to add the via mask
> clearance to the styles string. If the clearance are all zero (default),
> then it uses the old format so as to be backwards compatible.
>
> I haven't been able to test the lesstif hid yet... they updated
> something on my Mac and now Motif is seg faulting...
>
> Cheers,
> --Chad
>
> ** Changed in: pcb
> Status: Confirmed => In Progress
>

Chad Parker (parker-charles) wrote :

Dr. Mitch-

It's perfectly possible to run pcb out of the source tree. So, you can build it and test it without installing it (don't do the "make install" step. Thus, it remains entirely parallel to your existing system, and shouldn't disrupt anything.

The way I've implemented it, when a file is saved, if the all the via mask values in the styles are set to zero, then it will save in the older format. The via mask is saved as the last parameter in the styles definition, so, if your parser can handle an additional field in the line, there should be no problem. If you're using str.split(" ") to break the parameters, then your output list will just be one element longer. The order of the parameters hasn't changed, so, no existing code should break.

Thanks,
--Chad

Dr M (drmcn) wrote :

Okay, thank you.  I will give that a try.

On 03/25/2018 09:05 AM, Chad Parker wrote:
> Dr. Mitch-
>
> It's perfectly possible to run pcb out of the source tree. So, you can
> build it and test it without installing it (don't do the "make install"
> step. Thus, it remains entirely parallel to your existing system, and
> shouldn't disrupt anything.
>
> The way I've implemented it, when a file is saved, if the all the via
> mask values in the styles are set to zero, then it will save in the
> older format. The via mask is saved as the last parameter in the styles
> definition, so, if your parser can handle an additional field in the
> line, there should be no problem. If you're using str.split(" ") to
> break the parameters, then your output list will just be one element
> longer. The order of the parameters hasn't changed, so, no existing code
> should break.
>
> Thanks,
> --Chad
>

Chad Parker (parker-charles) wrote :

I started looking at why MinMaskGap wasn't working, and here's what I've found out.

There are presently two other avenues for affecting the soldermask clearance of vias.

1. ChangeClearSize
Enable the soldermask layer, select the vias you want to affect, then execute ChangeClearSize(SelectedVias, 0.5 mm) to set the soldermask clearance for all of the selected vias. Note that specifying SelectedVias will cause it to only affect vias. So, if you want to do all of them, you can just select everything on the board, and only the vias will be changed. There are other similar specifiers for other types of objects.

2. MinMaskGap
This action **only operates on vias that already have a non-zero mask gap** set. Also, this action only increases the mask gap if it's less than the specified value. If the mask is already greater than that value, the mask is not changed.

--Chad

Changed in pcb:
assignee: nobody → Chad Parker (parker-charles)
Chad Parker (parker-charles) wrote :

One thing we need to decide before this fix is released is what the value in this field should actually mean. It could be:

* the absolute diameter of the aperture,
* the difference in radius between the clearance aperture and the copper ring,
* the difference in radius between the clearance aperture and the drill hole

I think the way I've implemented it presently, it's the absolute diameter of the aperture, which is the value that's stored in pcb files. Since you don't always want to have any clearance, this might make the most sense, however, it's not what I'm used to.

FWIW, polygon clearance is stored as the difference in radius between the copper ring and the aperture in the polygon. So, when you say a clearance of 20 mils, there will be 20 mils of separation between the two copper objects.

Dr M (drmcn) wrote :

I think I like the absolute diameter.  In general, the parameters based
on differences for pads and vias are confusing.

On 04/01/2018 01:28 PM, Chad Parker wrote:
> One thing we need to decide before this fix is released is what the
> value in this field should actually mean. It could be:
>
> * the absolute diameter of the aperture,
> * the difference in radius between the clearance aperture and the copper ring,
> * the difference in radius between the clearance aperture and the drill hole
>
> I think the way I've implemented it presently, it's the absolute
> diameter of the aperture, which is the value that's stored in pcb files.
> Since you don't always want to have any clearance, this might make the
> most sense, however, it's not what I'm used to.
>
> FWIW, polygon clearance is stored as the difference in radius between
> the copper ring and the aperture in the polygon. So, when you say a
> clearance of 20 mils, there will be 20 mils of separation between the
> two copper objects.
>

Chad Parker (parker-charles) wrote :

The reason I hesitate on that is the word "clearance". Maybe it's not what other people call it, but I've always called it "solder mask clearance". And the word clearance makes me think that it's a difference.

Have you been able to test out the branch?

Dr M (drmcn) wrote :

Sorry, not yet, very busy. I have two design mods to do, but haven't
gotten to them yet.

On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden> wrote:

> The reason I hesitate on that is the word "clearance". Maybe it's not
> what other people call it, but I've always called it "solder mask
> clearance". And the word clearance makes me think that it's a
> difference.
>
> Have you been able to test out the branch?
>
> --
> You received this bug notification because you are subscribed to the bug
> report.
> https://bugs.launchpad.net/bugs/1744832
>
> Title:
> Vias tented
>
> Status in pcb:
> In Progress
>
> Bug description:
> Vias are created tented. So far, I have not found any description in
> the manual of to how to change this behavior, nor any description of
> how to un-tent the via once it has been created. I did see a mention
> in a blog that there is keyboard shortcut, "k", this does not seem to
> work. I have been correcting this manually by editing the PCB file.
>
> To manage notifications about this bug go to:
> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>

Dr M (drmcn) wrote :

I think I can get to it later today, will try

On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:

> Sorry, not yet, very busy. I have two design mods to do, but haven't
> gotten to them yet.
>
> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden> wrote:
>
>> The reason I hesitate on that is the word "clearance". Maybe it's not
>> what other people call it, but I've always called it "solder mask
>> clearance". And the word clearance makes me think that it's a
>> difference.
>>
>> Have you been able to test out the branch?
>>
>> --
>> You received this bug notification because you are subscribed to the bug
>> report.
>> https://bugs.launchpad.net/bugs/1744832
>>
>> Title:
>> Vias tented
>>
>> Status in pcb:
>> In Progress
>>
>> Bug description:
>> Vias are created tented. So far, I have not found any description in
>> the manual of to how to change this behavior, nor any description of
>> how to un-tent the via once it has been created. I did see a mention
>> in a blog that there is keyboard shortcut, "k", this does not seem to
>> work. I have been correcting this manually by editing the PCB file.
>>
>> To manage notifications about this bug go to:
>> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>>
>

Chad Parker (parker-charles) wrote :

There's no real rush, but testing is very much appreciated :) Don't
hesitate to ask if you have any questions.

On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden> wrote:

> I think I can get to it later today, will try
>
> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
>
> > Sorry, not yet, very busy. I have two design mods to do, but haven't
> > gotten to them yet.
> >
> > On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
> wrote:
> >
> >> The reason I hesitate on that is the word "clearance". Maybe it's not
> >> what other people call it, but I've always called it "solder mask
> >> clearance". And the word clearance makes me think that it's a
> >> difference.
> >>
> >> Have you been able to test out the branch?
> >>
> >> --
> >> You received this bug notification because you are subscribed to the bug
> >> report.
> >> https://bugs.launchpad.net/bugs/1744832
> >>
> >> Title:
> >> Vias tented
> >>
> >> Status in pcb:
> >> In Progress
> >>
> >> Bug description:
> >> Vias are created tented. So far, I have not found any description in
> >> the manual of to how to change this behavior, nor any description of
> >> how to un-tent the via once it has been created. I did see a mention
> >> in a blog that there is keyboard shortcut, "k", this does not seem to
> >> work. I have been correcting this manually by editing the PCB file.
> >>
> >> To manage notifications about this bug go to:
> >> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
> >>
> >
>
> --
> You received this bug notification because you are subscribed to the bug
> report.
> https://bugs.launchpad.net/bugs/1744832
>
> Title:
> Vias tented
>
> Status in pcb:
> In Progress
>
> Bug description:
> Vias are created tented. So far, I have not found any description in
> the manual of to how to change this behavior, nor any description of
> how to un-tent the via once it has been created. I did see a mention
> in a blog that there is keyboard shortcut, "k", this does not seem to
> work. I have been correcting this manually by editing the PCB file.
>
> To manage notifications about this bug go to:
> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>

Changed in pcb:
milestone: pcb-4.1.1 → pcb-4.2.0
Chad Parker (parker-charles) wrote :

Have you had the opportunity to test this at all?

Dr M (drmcn) wrote :
Download full text (3.1 KiB)

Hi Chad,

I am doing some PCB designs again.  So, we are at long last testing.
Our email chain listed below.

Per your suggestion, I fetched fresh versions of geda-gaf and pcb
(version v4.1.1-g3bcbb1c6) from git and built them in my directory
tree.   I have a few designs to generate in the next few days.

The "k" function seems to work admirably well, the solder mask enlarges
and reduces (shift k) around pads and pins, without a glitch.  Its a
very nice function actually.

(The gschem program however has some serious bugs, it crashes sporadically.)

Meanwhile, I have a new question.  For a surface mount part,  which
parameter is it that I want to reduce to allow a pad to connect to a
copper "pour" on the same side as the part.  I drew the "pours" on the
top surface with the rectangle tool, but the parts have some pads have
some space around them

Thank you

Mitch

On 04/02/2018 08:58 AM, Chad Parker wrote:
> There's no real rush, but testing is very much appreciated :) Don't
> hesitate to ask if you have any questions.
>
> On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden> wrote:
>
>> I think I can get to it later today, will try
>>
>> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
>>
>>> Sorry, not yet, very busy. I have two design mods to do, but haven't
>>> gotten to them yet.
>>>
>>> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
>> wrote:
>>>> The reason I hesitate on that is the word "clearance". Maybe it's not
>>>> what other people call it, but I've always called it "solder mask
>>>> clearance". And the word clearance makes me think that it's a
>>>> difference.
>>>>
>>>> Have you been able to test out the branch?
>>>>
>>>> --
>>>> You received this bug notification because you are subscribed to the bug
>>>> report.
>>>> https://bugs.launchpad.net/bugs/1744832
>>>>
>>>> Title:
>>>> Vias tented
>>>>
>>>> Status in pcb:
>>>> In Progress
>>>>
>>>> Bug description:
>>>> Vias are created tented. So far, I have not found any description in
>>>> the manual of to how to change this behavior, nor any description of
>>>> how to un-tent the via once it has been created. I did see a mention
>>>> in a blog that there is keyboard shortcut, "k", this does not seem to
>>>> work. I have been correcting this manually by editing the PCB file.
>>>>
>>>> To manage notifications about this bug go to:
>>>> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>>>>
>> --
>> You received this bug notification because you are subscribed to the bug
>> report.
>> https://bugs.launchpad.net/bugs/1744832
>>
>> Title:
>> Vias tented
>>
>> Status in pcb:
>> In Progress
>>
>> Bug description:
>> Vias are created tented. So far, I have not found any description in
>> the manual of to how to change this behavior, nor any description of
>> how to un-tent the via once it has been created. I did see a mention
>> in a blog that there is keyboard shortcut, "k", this does not seem to
>> work. I have been correcting this manually by editing the PCB file.
>>
>> To manage notifications about this bug go to:
>> https://bugs.launchpad.net/pcb/+bug/1744832/+subscri...

Read more...

Dr M (drmcn) wrote :
Download full text (3.6 KiB)

I think I figured out the answer to my question.  Is it 'ctrl-shift-k' ?

In a version where the functions are working, it really is a nice
program.  The documentation needs some work.  The recurring problem
seems to widespread use of abbreviated instructions and locally
undefined terms.

On 05/15/2018 06:01 PM, Dr M C Nelson wrote:
> Hi Chad,
>
> I am doing some PCB designs again.  So, we are at long last testing.
> Our email chain listed below.
>
> Per your suggestion, I fetched fresh versions of geda-gaf and pcb
> (version v4.1.1-g3bcbb1c6) from git and built them in my directory
> tree.   I have a few designs to generate in the next few days.
>
> The "k" function seems to work admirably well, the solder mask
> enlarges and reduces (shift k) around pads and pins, without a
> glitch.  Its a very nice function actually.
>
> (The gschem program however has some serious bugs, it crashes
> sporadically.)
>
> Meanwhile, I have a new question.  For a surface mount part, which
> parameter is it that I want to reduce to allow a pad to connect to a
> copper "pour" on the same side as the part.  I drew the "pours" on the
> top surface with the rectangle tool, but the parts have some pads have
> some space around them
>
> Thank you
>
> Mitch
>
> On 04/02/2018 08:58 AM, Chad Parker wrote:
>> There's no real rush, but testing is very much appreciated :) Don't
>> hesitate to ask if you have any questions.
>>
>> On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden> wrote:
>>
>>> I think I can get to it later today, will try
>>>
>>> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
>>>
>>>> Sorry, not yet, very busy.  I have two design mods to do, but haven't
>>>> gotten to them yet.
>>>>
>>>> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
>>> wrote:
>>>>> The reason I hesitate on that is the word "clearance". Maybe it's not
>>>>> what other people call it, but I've always called it "solder mask
>>>>> clearance". And the word clearance makes me think that it's a
>>>>> difference.
>>>>>
>>>>> Have you been able to test out the branch?
>>>>>
>>>>> --
>>>>> You received this bug notification because you are subscribed to
>>>>> the bug
>>>>> report.
>>>>> https://bugs.launchpad.net/bugs/1744832
>>>>>
>>>>> Title:
>>>>>    Vias tented
>>>>>
>>>>> Status in pcb:
>>>>>    In Progress
>>>>>
>>>>> Bug description:
>>>>>    Vias are created tented.  So far, I have not found any
>>>>> description in
>>>>>    the manual of to how to change this behavior, nor any
>>>>> description of
>>>>>    how to un-tent the via once it has been created.  I did see a
>>>>> mention
>>>>>    in a blog that there is keyboard shortcut, "k", this does not
>>>>> seem to
>>>>>    work. I have been correcting this manually by editing the PCB
>>>>> file.
>>>>>
>>>>> To manage notifications about this bug go to:
>>>>> https://bugs.launchpad.net/pcb/+bug/1744832/+subscriptions
>>>>>
>>> --
>>> You received this bug notification because you are subscribed to the
>>> bug
>>> report.
>>> https://bugs.launchpad.net/bugs/1744832
>>>
>>> Title:
>>>    Vias tented
>>>
>>> Status in pcb:
>>>    In Progress
>>>
>>> Bug descripti...

Read more...

Chad Parker (parker-charles) wrote :
Download full text (4.6 KiB)

Are you familiar with the thermal tool?

On Tue, May 15, 2018, 18:41 Dr M <email address hidden> wrote:

> I think I figured out the answer to my question. Is it 'ctrl-shift-k' ?
>
> In a version where the functions are working, it really is a nice
> program. The documentation needs some work. The recurring problem
> seems to widespread use of abbreviated instructions and locally
> undefined terms.
>
>
> On 05/15/2018 06:01 PM, Dr M C Nelson wrote:
> > Hi Chad,
> >
> > I am doing some PCB designs again. So, we are at long last testing.
> > Our email chain listed below.
> >
> > Per your suggestion, I fetched fresh versions of geda-gaf and pcb
> > (version v4.1.1-g3bcbb1c6) from git and built them in my directory
> > tree. I have a few designs to generate in the next few days.
> >
> > The "k" function seems to work admirably well, the solder mask
> > enlarges and reduces (shift k) around pads and pins, without a
> > glitch. Its a very nice function actually.
> >
> > (The gschem program however has some serious bugs, it crashes
> > sporadically.)
> >
> > Meanwhile, I have a new question. For a surface mount part, which
> > parameter is it that I want to reduce to allow a pad to connect to a
> > copper "pour" on the same side as the part. I drew the "pours" on the
> > top surface with the rectangle tool, but the parts have some pads have
> > some space around them
> >
> > Thank you
> >
> > Mitch
> >
> > On 04/02/2018 08:58 AM, Chad Parker wrote:
> >> There's no real rush, but testing is very much appreciated :) Don't
> >> hesitate to ask if you have any questions.
> >>
> >> On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden>
> wrote:
> >>
> >>> I think I can get to it later today, will try
> >>>
> >>> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
> >>>
> >>>> Sorry, not yet, very busy. I have two design mods to do, but haven't
> >>>> gotten to them yet.
> >>>>
> >>>> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
> >>> wrote:
> >>>>> The reason I hesitate on that is the word "clearance". Maybe it's not
> >>>>> what other people call it, but I've always called it "solder mask
> >>>>> clearance". And the word clearance makes me think that it's a
> >>>>> difference.
> >>>>>
> >>>>> Have you been able to test out the branch?
> >>>>>
> >>>>> --
> >>>>> You received this bug notification because you are subscribed to
> >>>>> the bug
> >>>>> report.
> >>>>> https://bugs.launchpad.net/bugs/1744832
> >>>>>
> >>>>> Title:
> >>>>> Vias tented
> >>>>>
> >>>>> Status in pcb:
> >>>>> In Progress
> >>>>>
> >>>>> Bug description:
> >>>>> Vias are created tented. So far, I have not found any
> >>>>> description in
> >>>>> the manual of to how to change this behavior, nor any
> >>>>> description of
> >>>>> how to un-tent the via once it has been created. I did see a
> >>>>> mention
> >>>>> in a blog that there is keyboard shortcut, "k", this does not
> >>>>> seem to
> >>>>> work. I have been correcting this manually by editing the PCB
> >>>>> file.
> >>>>>
> >>>>> To manage notifications about this bug go to:
> >>>>> https://bugs.launchpad.net/pcb/+bug/1744832/+subscrip...

Read more...

Dr M (drmcn) wrote :
Download full text (5.0 KiB)

Yes,of course.   It did nothing.

The "pours" are drawn on the top of the board using the rectangle and
polygon tools. Its a "one layer" board.

I tried the thermal, but nothing happened.  But,  after ctl-shift-k, the
rats net shows everything is connected.

On 05/15/2018 06:47 PM, Chad Parker wrote:
> Are you familiar with the thermal tool?
>
> On Tue, May 15, 2018, 18:41 Dr M <email address hidden> wrote:
>
>> I think I figured out the answer to my question. Is it 'ctrl-shift-k' ?
>>
>> In a version where the functions are working, it really is a nice
>> program. The documentation needs some work. The recurring problem
>> seems to widespread use of abbreviated instructions and locally
>> undefined terms.
>>
>>
>> On 05/15/2018 06:01 PM, Dr M C Nelson wrote:
>>> Hi Chad,
>>>
>>> I am doing some PCB designs again. So, we are at long last testing.
>>> Our email chain listed below.
>>>
>>> Per your suggestion, I fetched fresh versions of geda-gaf and pcb
>>> (version v4.1.1-g3bcbb1c6) from git and built them in my directory
>>> tree. I have a few designs to generate in the next few days.
>>>
>>> The "k" function seems to work admirably well, the solder mask
>>> enlarges and reduces (shift k) around pads and pins, without a
>>> glitch. Its a very nice function actually.
>>>
>>> (The gschem program however has some serious bugs, it crashes
>>> sporadically.)
>>>
>>> Meanwhile, I have a new question. For a surface mount part, which
>>> parameter is it that I want to reduce to allow a pad to connect to a
>>> copper "pour" on the same side as the part. I drew the "pours" on the
>>> top surface with the rectangle tool, but the parts have some pads have
>>> some space around them
>>>
>>> Thank you
>>>
>>> Mitch
>>>
>>> On 04/02/2018 08:58 AM, Chad Parker wrote:
>>>> There's no real rush, but testing is very much appreciated :) Don't
>>>> hesitate to ask if you have any questions.
>>>>
>>>> On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden>
>> wrote:
>>>>> I think I can get to it later today, will try
>>>>>
>>>>> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
>>>>>
>>>>>> Sorry, not yet, very busy. I have two design mods to do, but haven't
>>>>>> gotten to them yet.
>>>>>>
>>>>>> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
>>>>> wrote:
>>>>>>> The reason I hesitate on that is the word "clearance". Maybe it's not
>>>>>>> what other people call it, but I've always called it "solder mask
>>>>>>> clearance". And the word clearance makes me think that it's a
>>>>>>> difference.
>>>>>>>
>>>>>>> Have you been able to test out the branch?
>>>>>>>
>>>>>>> --
>>>>>>> You received this bug notification because you are subscribed to
>>>>>>> the bug
>>>>>>> report.
>>>>>>> https://bugs.launchpad.net/bugs/1744832
>>>>>>>
>>>>>>> Title:
>>>>>>> Vias tented
>>>>>>>
>>>>>>> Status in pcb:
>>>>>>> In Progress
>>>>>>>
>>>>>>> Bug description:
>>>>>>> Vias are created tented. So far, I have not found any
>>>>>>> description in
>>>>>>> the manual of to how to change this behavior, nor any
>>>>>>> description of
>>>>>>> how to un-tent the via once it has been created. I did...

Read more...

Dr M (drmcn) wrote :
Download full text (4.9 KiB)

Re the thermal tool suggestion.  I found the problem.   We are talking
about connecting pads for an SMT part to a copper pour. According the
documentation, the tool will make a thermal for a pin or via, not for a pad.

On 05/15/2018 06:47 PM, Chad Parker wrote:
> Are you familiar with the thermal tool?
>
> On Tue, May 15, 2018, 18:41 Dr M <email address hidden> wrote:
>
>> I think I figured out the answer to my question. Is it 'ctrl-shift-k' ?
>>
>> In a version where the functions are working, it really is a nice
>> program. The documentation needs some work. The recurring problem
>> seems to widespread use of abbreviated instructions and locally
>> undefined terms.
>>
>>
>> On 05/15/2018 06:01 PM, Dr M C Nelson wrote:
>>> Hi Chad,
>>>
>>> I am doing some PCB designs again. So, we are at long last testing.
>>> Our email chain listed below.
>>>
>>> Per your suggestion, I fetched fresh versions of geda-gaf and pcb
>>> (version v4.1.1-g3bcbb1c6) from git and built them in my directory
>>> tree. I have a few designs to generate in the next few days.
>>>
>>> The "k" function seems to work admirably well, the solder mask
>>> enlarges and reduces (shift k) around pads and pins, without a
>>> glitch. Its a very nice function actually.
>>>
>>> (The gschem program however has some serious bugs, it crashes
>>> sporadically.)
>>>
>>> Meanwhile, I have a new question. For a surface mount part, which
>>> parameter is it that I want to reduce to allow a pad to connect to a
>>> copper "pour" on the same side as the part. I drew the "pours" on the
>>> top surface with the rectangle tool, but the parts have some pads have
>>> some space around them
>>>
>>> Thank you
>>>
>>> Mitch
>>>
>>> On 04/02/2018 08:58 AM, Chad Parker wrote:
>>>> There's no real rush, but testing is very much appreciated :) Don't
>>>> hesitate to ask if you have any questions.
>>>>
>>>> On Mon, Apr 2, 2018 at 8:35 AM, Dr M <email address hidden>
>> wrote:
>>>>> I think I can get to it later today, will try
>>>>>
>>>>> On Mon, Apr 2, 2018, 8:35 AM M Nelson <email address hidden> wrote:
>>>>>
>>>>>> Sorry, not yet, very busy. I have two design mods to do, but haven't
>>>>>> gotten to them yet.
>>>>>>
>>>>>> On Mon, Apr 2, 2018, 8:25 AM Chad Parker <email address hidden>
>>>>> wrote:
>>>>>>> The reason I hesitate on that is the word "clearance". Maybe it's not
>>>>>>> what other people call it, but I've always called it "solder mask
>>>>>>> clearance". And the word clearance makes me think that it's a
>>>>>>> difference.
>>>>>>>
>>>>>>> Have you been able to test out the branch?
>>>>>>>
>>>>>>> --
>>>>>>> You received this bug notification because you are subscribed to
>>>>>>> the bug
>>>>>>> report.
>>>>>>> https://bugs.launchpad.net/bugs/1744832
>>>>>>>
>>>>>>> Title:
>>>>>>> Vias tented
>>>>>>>
>>>>>>> Status in pcb:
>>>>>>> In Progress
>>>>>>>
>>>>>>> Bug description:
>>>>>>> Vias are created tented. So far, I have not found any
>>>>>>> description in
>>>>>>> the manual of to how to change this behavior, nor any
>>>>>>> description of
>>>>>>> how to un-tent the via once it has been created. I did see a
>>>>>>> mention
>>>>>>> in a b...

Read more...

To post a comment you must log in.
This report contains Public information  Edit
Everyone can see this information.

Other bug subscribers

Related blueprints