Mail Archives: geda-user/2013/09/18/15:17:04
Rob,
You can indeed put a gschemrc into each project to handle stuff that is
project specific. However, you can also have a per-user gschemrc in
you're home directory. If you put the file there, it will work for all
projects that you create and anything in the project's gschemrc will
take precedence if there is a conflict. If anyone else uses the system,
they have their own gschemrc to customize as they please. I haven't
done much with system-gschemrc, other than to customize it by
adding/subtracting comments. If you really need to change it, you'll
have to change the access privileges with sudo chmod to be world
writeable. Just remember to change them back when finished and to save a
copy of the original file. You may just break gschem by changing
something in this file and then not remember exactly what it was changed
from. I would really recommend using /home/yourUserName/.gEDA/gschemrc.
The only time I would use system-gschemrc is in the case where there are
multiple users that all need to be constrained to use the same settings
for consistency across the group.
On 09/18/2013 03:04 PM, Rob Butts wrote:
> I'd like to change the system-gschemrc file if I can ~ this way I don't
> have to make up new gschemrc files for each project. It is read only. Can
> I place a gshcemrc file in the gaf folder and have it for all subfolders?
>
>
> On Wed, Sep 18, 2013 at 2:22 PM, Rob Butts <r DOT butts2 AT gmail DOT com> wrote:
>
>> Great!
>>
>> Thanks!
>>
>>
>> On Wed, Sep 18, 2013 at 2:15 PM, Stephen R. Besch <sbesch AT buffalo DOT edu>wrote:
>>
>>> Rob,
>>>
>>> I should also mention that I find the easiest way to generate a new
>>> symbol from an old one is to insert the old one onto a schematic, select it
>>> and click on the Hierarchy...Down Symbol command from the top menu bar.
>>> Then use the File menu to save the symbol in your local library, probably
>>> with a new name. Type "en" followed by "et" (and accept the Translation
>>> entry box that results from the "et" command.
>>>
>>> Now you can edit the symbol to you're hearts content. When done, hit "en"
>>> followed by "et" to re-hide hidden attributes and translate the symbol back
>>> to 0, save a final time and you're almost done.
>>> Before you lose track of it, use the hierarchy UP command to return to
>>> the main schematic and delete the now unneeded "old" symbol.
>>>
>>> Note that gschem won't see the new symbol until after the next restart.
>>>
>>>
>>> On 09/18/2013 02:01 PM, Rob Butts wrote:
>>>
>>>> Thanks!
>>>>
>>>> I know where the resistor symbols are in gschem. Now I now where the
>>>> symbol file is.
>>>>
>>>> Thanks for showing me how to add the attributes!
>>>>
>>>>
>>>> On Wed, Sep 18, 2013 at 1:39 PM, Stephen R. Besch <sbesch AT buffalo DOT edu
>>>>> wrote:
>>>> On 09/18/2013 01:16 PM, Rob Butts wrote:
>>>>> I know this is a much discussed subject but I haven't followed it much
>>>>>> and
>>>>>> reading the results of a search is confusing this non-guru-linux user.
>>>>>>
>>>>>> I was just about to locate the resistor symbol to make my own version
>>>>>> with
>>>>>> attributes of footprint, part number, digikey part number...
>>>>>>
>>>>>> Does this exist?
>>>>>>
>>>>>> There are 2 questions posed here. First, is there a symbol for a
>>>>>>
>>>>> resistor in the standard library? Yes there is. Look in the MISC
>>>>> category
>>>>> and pick one of those as a staring point. The other question is: Does
>>>>> any
>>>>> one already have such a customized resistor symbol? The answer to this
>>>>> is
>>>>> also yes. However, since attribute preferences and component style will
>>>>> differ, you're probably better off rolling your own. I would also
>>>>> suggest
>>>>> that you add your custom attributes to the gschemrc file located the
>>>>> .gEDA
>>>>> folder found in your home directory. Then when you click on the
>>>>> attribute
>>>>> Drop down when adding an attribute, your custom choices will be there.
>>>>> This has 2 advantages: 1) You don't have to type them every time, and
>>>>> 2)
>>>>> it avoids having slight differences in the spelling of the attributes
>>>>> when
>>>>> constructing parts.
>>>>>
>>>>> gschemrc is also where you define the location of your custom component
>>>>> library(s). So, you would add something like this:
>>>>>
>>>>> (component-library "${HOME}/gaf/your_local-sym_****directory")
>>>>>
>>>>>
>>>>> (attribute-name "Vendor")
>>>>> (attribute-name "VendorPN")
>>>>> (attribute-name "Manufacturer")
>>>>>
>>>>>
>>>>> --
>>>>> fictio cedit veritati
>>>>>
>>>>>
>>>>>
>>> --
>>> fictio cedit veritati
>>>
>>>
--
fictio cedit veritati
- Raw text -