kicad-developers team mailing list archive

[Cirilo Bernardo <cirilo.bernardo@xxxxxxxxx>]

Thanks Maurice,

 Maybe you should also post to the user list. I'm sure everyone who needs
solid models will find it useful and you would get more testing done as
well; I'm finding it very difficult to find time to do even simple testing
at the moment and I haven't built FreeCAD for a few years now so I only
have what's available on Debian (0.14).

 This looks very good and will be very useful and is much less hassle than
the process which many people use to convert their VRML models to a solid
model. It will still be many months yet before KiCad has a native solid
model export which I'm guessing will be IGES at this point, and who knows
how much longer it will be before someone finds time to add STEP. The
combination of IDF + STEP is good since the solid model of the PCB will
actually have circular drill holes which can be used by MCADs as a
reference point; models derived from VRML rendering of the board always
give polygonal holes which are frustrating to work with in MCAD.

- Cirilo


On Fri, Jul 3, 2015 at 7:08 PM, easyw <easyw@xxxxxxxxxxxx> wrote:

> Hi Cirilo,
>
> I've uploaded the recent version of the script with the demo board at
> sourceforge
> https://sourceforge.net/projects/kicadstepup/?source=navbar
> (I know I should have done in launchpad but I'm not familiar with bzr
> etc... I promise I will learn it)
> In the updated script I've put some check for the presence of files and
> models, so to give messages to the user...
>
> there is a readme file
> http://sourceforge.net/projects/kicadstepup/files/README.txt/download
> and the demo folder with all files
>
> http://sourceforge.net/projects/kicadstepup/files/kicad_StepUp_v0.42.zip/download
>
> the script is a python script for freecad (kicad_StepUp.FCMacro)
>
> just move to the demo dir and launch
>    freecad demo.emn kicad_StepUp.FCMacro
> (the demo.emn is the IDF file exported through your IDF routines)
>
> here there is also a link of the script in action...
> http://youtu.be/Ukd47VXYzQU
>
> the trick to obtain the hierarchical STEP file from freecad 0.15 is to use
> export 'STEP with colors' from File menu (NOT from Part menu)
>
> Please have a try at the demo and eventually with some of your kicad
> projects and let me know your feedback ...
>
> thank you
> Maurice
>
> On 03/07/2015 00.39, Cirilo Bernardo wrote:
>
>> Hi Maurice,
>>
>>   This is good in SolidWorks as well; I have a few questions:
>>
>> Where is this FreeCAD script to process the files and create the assembly?
>>
>> What is the secret to making OCC/FreeCAD create a hierarchical STEP file
>> rather than a flat file?
>>
>> - Ciirlo
>>
>> On Thu, Jul 2, 2015 at 7:28 PM, easyw <easyw@xxxxxxxxxxxx
>> <mailto:easyw@xxxxxxxxxxxx>> wrote:
>>
>>     @Tom
>>
>>     Hi Tom, following your advices (design in STEP B-Rep)
>>     I came with this approach:
>>     - prepare or just download STEP models for 3D parts
>>     - convert STEP to VRML to build the pcb in kicad (using FreeCAD)
>>     - just place pcb parts in kicad as always
>>     - export IDF pcb plain board
>>     - assembly automatically the board in MCAD reading 3D modules and
>>        positions from kicad pcb file with the kicad_StepUp script
>>     - export the STEP assembly from MCAD  (using FreeCAD)
>>
>>     I asked a friend of mine to import the result in SolidWorks and it
>>     seems to be fine...
>>
>>     Could you please check if the result (demo.step) it is fine in
>>     hierarchical STEP assembly?
>>
>>     Thank you very much
>>     Maurice
>>
>>
>>
>>     On 01/07/2015 23.49, easyw wrote:
>>
>>         Hi,
>>
>>         kicad StepUp is a new approach to export kicad board and modules
>>         in STEP
>>         AP214 (with colors)
>>
>>         exporting needs these requirements:
>>         1) install FreeCAD 0.15
>>               1b) in windows copy the Idf.py patched file in
>> FreeCAD/Mod/Idf
>>         folder (in Linux IDF import seems fine)
>>         2) start your 3D module model design directly in STEP using
>>         FreeCAD or
>>         just getting the model from a STEP library
>>              (units mm required)
>>         3) put your STEP model in the same directory in which are
>>         normally the
>>         wrl models
>>         4) convert your 3D STEP model in vrml through FreeCAD
>>              (scaling it to 0.3937, a kicad_StepUp_vrml_export macro is
>>         provided
>>               just launch e.g. freecad sot23.step
>>         kicad_StepUp_vrml_export.FCMacro)
>>         4) in pcbnew just populate your board as usual, using only vrml
>>         models
>>         with the corresponding model in STEP
>>         5) export the plain board through IDF menu (no IDF models are
>>         needed,
>>         just wrl standard ones)
>>         6) move to the 'demo' dir and execute the python kicad_StepUp
>>         FCMacro
>>         launching:
>>            freecad demo.emn kicad_StepUp.FCMacro
>>            (in windows you may need to specify freecad.exe bin
>>             path)
>>         and wait until your 3D board will be automatically
>>         populated following kicad_pcb source board
>>         (note only kicad_pcb version 4 is supported)
>>         7) the script can be configured to follow the KISYS3DMOD path
>>
>>         Please consider that the project is at alpha state and not
>>         everything
>>         has been completed
>>         (e.g. at the moment Bottom items do not respect orientation,
>>            and Top orientation is referred only to pcb module, assuming
>> wrl
>>         module ha the same orientation
>>            the script will stop in case of missing modules without any
>>         message)
>>
>>         I would need someone to check if the models used and the resulting
>>         demo.step obtained from the elaboration
>>         is fine to be used in MCAD e.g. SolidWorks that I do not have...
>>         I checked the result with a trial of Catia and Rhino and it
>>         seems fine...
>>
>>         If the result is fine to be used in MCAD the refined script could
>> be
>>         used to convert the pcb artworks for 3D MCAD modelling, and could
>> be
>>         easily ready to go for the stable release....
>>
>>         The only requirements, different from the actual way of using
>>         kicad is
>>         to substitute Wings3D with FreeCAD and, obviously, populate the 3D
>>         models with STEP lib...
>>         (anyway Wings3D can be used besides FreeCAD if the 3D STEP
>>         exporting it
>>         is not needed)
>>
>>         attached a kicad demo project, with self containing STEP and wrl
>>         modules
>>         to be used just out of the box,
>>         some screen-shots of the result
>>         here there is also a link of the script in action...
>>         http://youtu.be/Ukd47VXYzQU
>>
>>         thank you for any suggestion and feedback,
>>         Maurice
>>
>>
>>     _______________________________________________
>>     Mailing list: https://launchpad.net/~kicad-developers
>>     Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>     <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>     Unsubscribe : https://launchpad.net/~kicad-developers
>>     More help   : https://help.launchpad.net/ListHelp
>>
>>
>>