kicad-developers team mailing list archive

["Jose A. Saumell" <saumell.jose@xxxxxxxxx>]

Hi Maurice, Cirilo and everyone,

Thanks for the advise.

I was able to run the demo with FreeCAD script, as was shown in youtube
video.

What I have now is a complete 3D model of my own board I can view on PCBnew
3D viewer. That looks fine and uses WRL models for each individual
component ( Usually downloaded and modified with FreeCAD and later Wings3D
for WRL.
I've generated an .emn file and run the macro, it gave me an error when it
could not find step files for components.

So, if I understand correctly, I would need two formats for each component,
WRL for kicad 3D viewer and step for the StepUp FreeCAD Macro, correct?.
Apparently going from VRML to STEP is not recommended so I should create
components in STEP format from FreeCAD.

Regarding documentation, I can tell you what my experience has been. I've
followed instructions to get a complete 3D model I could view with PCBnew,
assuming I was going to be able to export that to Solidworks somehow. For
kicad users maybe would be good to know STEP procedure before generating
all WRL models, or generating both at the same time.

It is the first time in my career that I attempt to generate a 3D model of
a PCB and interface with MCAD engineers this way.It is pretty exciting and
should save a lot of time in meetings.

Thanks!






On Wed, Aug 5, 2015 at 5:31 AM easyw <easyw@xxxxxxxxxxxx> wrote:

> Hi Saumell,
>
> When you need to give your 3d artwork to MCAD people you have to use
> step as interchange format.
> Any other format would not be accepted.
> Before the kicad stepup script the only way I know to export the pcb
> with models was to export vrml and then convert it to step; but any
> model converted from vrml would be very un-optimal and not very useful
> for mechanical design (I learned the hard way)... the conversion, using
> whatever sw you find, will generate a bunch of triangles.
>
> as Cirilo suggested, please have a try with kicad-stepup script:
> http://bazaar.launchpad.net/~easyw/kicad-stepup/trunk/files
> http://sourceforge.net/projects/kicadstepup/
> I'm going to write an howto to be included in kicad doc.
> At the moment the README.txt file gives you a small explanation.
> @youtube you can see also a small howto video
> https://www.youtube.com/watch?v=Ukd47VXYzQU
> I've also added the option to move the board and modules to a base
> point, and the bounding boxes option (to export all or selected modules
> to bbox)
>
> At the moment the kicad library lacks of STEP modules...
> I've suggested to add to the 3D repository at least models generated
> from FreeCAD
> https://github.com/KiCad/kicad-library/issues/186
> FreeCAD could be used as second source to model 3D object to kicad, side
> by side with wings3d.
> Moreover FreeCAD can create parametric model, with real dimensions as
> per the physical objects.
>
> Anyway, if you need just a rapid solution, you can get 3d models at
> http://3dcontentcentral.com/
> the only requirement for the script to work is to have the single models
> as a single fused object
> you can find some tips to align and use the modules here:
>
> https://forum.kicad.info/t/kicad-stepup-new-exporter-for-3d-mcad-feedbacks-are-welcome/1048
>
> To test the script in real world, I used hackrf-one board and I
> generated all 3d vrml modules to be used in kicad, directly from step
> modules downloaded from the manufacturers or from 3dcontent central
> library.
> All the modules converted from FreeCAD to wrl has been used in kicad
> 3d-viewer without any issue.
> The STEP generated model has been tested in Solid Works and it is fine
> without any geometry problem.
>
> Could you please give me a feed back of your test, so to improve the
> script usability for kicad users?
>
> thank you
> Maurice
>
> On 05/08/2015 00.17, Cirilo Bernardo wrote:
> > There are a number of options:
> >
> > 1. Recently Maurice wrote a script which uses FreeCAD to create a
> > STEP modelusing the bare board IDF file and other data in the
> > .kicad_pcb file:
> >
> > http://bazaar.launchpad.net/~easyw/kicad-stepup/trunk/files
> >
> > No doubt there are still some issues but this is currently the best
> > method for exporting a detailed mechanical model.
> >
> > 2. IDF: If you do nothing and simply opt to export the board then
> > you only get a bare board - this step is necessary anyway if you
> > use Maurice's script to create a STEP model. If you wish for a more
> > detailed IDF model you will need to spend some time creating the
> > associated component outline files.  The official IDF documentation
> > is here:
> >
> > https://github.com/ciampix/kicad-doc/tree/master/src/IDF_Exporter
> >
> > but if you can't generate the documentation and want a PDF version
> > the original (more inaccurate) version is here:
> >
> > https://drive.google.com/open?id=0By_XTJN-s8aXbkM5UTE0Zm5SN28
> >
> > Now for Solidworks to process an IDF file you need CircuitWorks which
> > is only provided with "Solidworks Premium" - bummer. Fortunately you
> > can now convert IDF to IGES (which any MCAD can understand) using
> > the 'idf2igs' tool in the IGES library which is in development:
> >
> > https://github.com/cbernardo/libIGES
> >
> > There are also online tools to help such as:
> > https://www.ecad.io
> >
> > That site provides all the functionality of CircuitWorks - you can
> > substitute real models for the simplistic IDF outlines. However, if the
> > simple IDF outlines are fine for your mechanical work then the
> > libIGES tool is a completely free solution.
> >
> > Expect more MCAD exchange features in the future, though the wait
> > may be a little long due to limited resources. My libIGES already has
> > the capability to create models of the bare PCB and to add other
> > existing IGES models to the mechanical assembly and I plan to add
> > an IGES export to KiCad some time after the pending stable release.
> > Unfortunately I also need to do some major work on the KiCad code
> > base before I add this code so it could be another 6 months or more
> > before you see that feature in KiCad. There have also been discussions
> > on adding a STEP export facility using the OpenCascade libraries,
> > but this is also dependent on those code changes which I need to
> > make to KiCad. So for now, Maurice's scripts are really the best
> > option for creating a detailed mechanical model.
> >
> > - Cirilo
> >
> >
> > On Wed, Aug 5, 2015 at 7:21 AM, Jose A. Saumell <saumell.jose@xxxxxxxxx
> > <mailto:saumell.jose@xxxxxxxxx>> wrote:
> >
> >     Hello group,
> >
> >     I have been trying to export a 3D model of a populated PCB to
> >     Solidworks and after a few days I want to ask you for help.
> >
> >     I've generated VRML files for each component and did an export in
> >     VRML which I can open and see in FreeCAD correctly.
> >
> >     I need to interface with Mechanical Engineer that has their own
> >     Solidworks model for the enclosure. He has been able to open the
> >     populated PCB on Freecad as well. (To achieve this I had to use a
> >     text editor and modify all the url entries on WRL file with an
> >     absolute path on his system containing shapes3D folder, at least
> >     freecad does not seem to work with relative path)
> >
> >     What he was able to achieve so far is opening the empty PCB in
> >     solidworks and load each individual component and placing manually
> >     on the board.
> >
> >     Is there any other way or tips you can provide? I've read about IDF
> >     and I may go that route with the next design if it means easier
> >     interfacing with Solidworks.
> >
> >     Thanks
> >
> >     _______________________________________________
> >     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
> >
> >
> >
> >
> > _______________________________________________
> > Mailing list: https://launchpad.net/~kicad-developers
> > Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> > Unsubscribe : https://launchpad.net/~kicad-developers
> > More help   : https://help.launchpad.net/ListHelp
> >
>