kicad-developers team mailing list archive

[easyw <easyw@xxxxxxxxxxxx>]

Hi Wayne,

sorry again ... I don't know why but I cannot attach also images...

ok I'm trying with adoc in plain text
and images with links


I've done a first kicad StepUp starting guide...

it is an asciidoc with some images (to put in images/ dir)

I attached the adoc+images links
image 1
http://www.kicad-pcb.org/download/attachments/589828/hackrf-one-stepup-kicad-3d-viewer.png
image 2
http://www.kicad-pcb.org/download/attachments/589828/hackrf-one-stepup-catia-assembly.png
image 3
https://raw.githubusercontent.com/easyw/kicad-3d-models-in-freecad/master/reference-block-imported.jpg

is it fine or should I do something else to add it to the doc repository?

thank you and sorry again for the 3 mails...
Maurice

On 05/08/2015 14.27, Wayne Stambaugh wrote:
> Maurice,
>
> I think Marco is currently on vacation.  The new documentation format is
> asciidoc.  You can use git to clone the current documentation at
> https://github.com/ciampix/kicad-doc.  Information on how to use
> asciidoc can be found at http://www.methods.co.nz/asciidoc/
>
> Wayne
>
> On 8/5/2015 8:23 AM, easyw wrote:
> > @Marco
> >
> > what could I do to prepare a small tutorial for the kicad stepup script?
> > do you accept libre-office file or pdf file?
> > I'm sorry but I'm new to the doc side :)
> >
> > thank you
> > Maurice
> >
> > On 17/07/2015 15.12, Wayne Stambaugh wrote:
> > > On 7/17/2015 3:36 AM, Mário Luzeiro wrote:
> > > > Excellent!
> > > >
> > > > Do you (all) think should be nice to have a small step tutorial /
> > > > explanation how can someone reproduce identical results for another
> > > > boards?
> > >
> > > Yes.  Any help we can provide our users is a good thing.  Something like
> > > this should be added to the user documentation either as part of the
> > > Pcbnew manual or as a stand alone tutorial.  I don't have a preference
> > > one way or another so I'll leave that decision to our documentation
> > > experts.
> > >
> > > > Mario Luzeiro


Kicad StepUp starter Guide
==========================
:Author:    Maurice
:Email:     https://launchpad.net/~easyw
:Author Initials: MEW
:Date:      August 2015
:Revision:  1.1
:website: http://sourceforge.net/projects/kicadstepup/
:docname: readme-kicadStepUp.adoc

kicad StepUp: a new approach to export kicad board and modules in STEP AP214 (with colors).
With kicad StepUp it is possible to export the 3D board and modules in STEP
for MCAD interchange and create the 3D wrl libraries. +

link:http://sourceforge.net/projects/kicadstepup/[kicadStepUp at sourceforge] +
link:http://bazaar.launchpad.net/~easyw/kicad-stepup/trunk/files/[kicadStepUp at lauchpad]

.OverView
**********************************************************************
to run the demo:

in Linux:
change dir to the folder in which you have extracted the demo +
./launch-kicad_StepUp-demo.sh

in windows:
change dir to the folder in which you have extracted the demo +
launch-kicad_StepUp-demo.bat

the demo comes with a kicad project, along with all needed STEP and wrl modules, just to be used just out of the box +
(*NB* use the script from inside the dir)

here there is also a link of the script in action... +
link:http://youtu.be/Ukd47VXYzQU[YouTube Kicad StepUp demo video]

*requirements:*
kicad 2015 stable or latest dev release, freecad 0.15
**********************************************************************

Introduction
------------
Kicad StepUp allows the user to modeling the 3D modules starting from FreeCAD
(instead of using Wings3D), creating models in STEP AP214 and rendering the
pcb board and components in native STEP AP214.

Designing in kicad native 3d-viewer will produce a fully aligned STEP version
with the same view of kicad 3d render. +
Now you will have the two words with the same appearance; one can design in kicad EDA and transfer the artwork to MCAD (FreeCAD) smoothly

*WYSIWYG from EDA to MCAD*

.kicad StepUp in Kicad 3d-viewer
image::images/hackrf-one-stepup-kicad-3d-viewer.png[]

.kicad StepUp in MCAD Catia
image::images/hackrf-one-stepup-catia-assembly.png[]

Basic How To '(using kicad StepUp the easiest way)'
---------------------------------------------------

*(not changing the way you use kicad)*

*1.* just copy the STEP 3d models in the same folder in which there are your wrl 3d models and
   use the same name of the wrl model name (e.g. r_0603.wrl => r_0603.step) +
*2.* go to your board folder and copy the script kicad_StepUp.FCMacro and the config file ksu-config.cfg
   inside that folder, edit the config file ksu-config.cfg with e.g. notepad changing your model prefix to your KISYS3DMOD path +
*3.* export from kicad pcbnew the IDF model of the board +
*4.* run the script from command line or from a bash/batch file +
    <path to Freecad executable file>/freecad <kicad_pcb_name.emn> ksu-config.cfg kicad_StepUp.FCMacro +
    '(e.g. freecad mypcb.emn ksu-config.cfg kicad_StepUp.FCMacro)' +
*just watch the script assembly your 3D board with 3D models :)*

How To '(using kicad StepUp the best way)'
------------------------------------------

*(getting the best from STEP models)*

*1.* just copy the STEP 3d models in the same folder in which there are your wrl 3d models +
*2.* export the STEP models, scaled 1/2.54 to wrl with the same name of the STEP model
(e.g. r_0603.wrl => r_0603.step); in this way your 3D board in kicad pcbnew 3d-viewer and in FreeCAD workbench will look perfectly aligned +
*3.* go to your board folder and copy the script kicad_StepUp.FCMacro and the config file ksu-config.cfg
   inside that folder, edit the config file ksu-config.cfg with e.g. notepad changing your model prefix to your KISYS3DMOD path +
*4.* export from kicad pcbnew the IDF model of the board +
*5.* run the script from command line or from a bash/batch file +
    <path to Freecad executable file>/freecad <kicad_pcb_name.emn> ksu-config.cfg kicad_StepUp.FCMacro +
    '(e.g. freecad mypcb.emn ksu-config.cfg kicad_StepUp.FCMacro)' +
*just watch the script assembly your 3D board with 3D models :)*

Create your own Library
----------------------

The way to build a STEP models library to be easily used by the script is:

- start modeling your 3d object in scale 1:1 in mm
(which is the way in which mechanical stuff are used to be)
- convert your model to STEP in scale 1:1
- assure that your STEP module *is fused to just one solid object*
- convert the model to wrl in scale 1/2.54 (0.3937001)
(which is the scale used by kicad 3d-viewer or maintain 1:1 scale in exporting and apply
the scale 1/2.54 to the wrl model in 3d-viewer)
- use the same name to wrl and STEP model
- put the STEP model and VRML model in the same place
- check if your vrml model is aligned to the kicad pcb footprint in pcbnew 3d-viewer
- launch the script and check if the FreeCAD model and the kicad 3D viewer are aligned
- in case of misalignment just verify your model

TIP: Tip. +
*import* the link:https://raw.githubusercontent.com/easyw/kicad-3d-models-in-freecad/master/reference-block.step[reference block] in your FC doc
beside the model you are designing to check the correct orientation +
(*NB Import Ctrl+I*, 'not Open Ctrl+O')

.reference block imported
image::images/reference-block-imported.jpg[]

*Note:* here link:http://forum.freecadweb.org/viewtopic.php?t=8451#p69489[FreeCAD forum fusion howto] some tips to fuse correctly objects in FreeCAD

STEP AP214 and VRML FreeCAD scripted repository ready to kicad StepUp
---------------------------------------------------------------------
link:https://github.com/easyw/kicad-3d-models-in-freecad[repository of 3D STEP models:] +
there is a repository of many electronic components *STEP AP214* models, with a nice script to build parametric models for
'SOIC, SSOP, TSSOP, SOT, QFP' ICs just compiling a parametric text file with dimensions from component data sheet

'more is coming ...'

credits
-------

'kicad StepUp' script author is {author} link:https://launchpad.net/~easyw/[easyw@launchpad] +
Guide Doc Version is {revision}

link:http://www.kicad-pcb.org/display/KICAD/KiCad+EDA+Software+Suite[kicad EDA] +
- IDF export for kicad (Cirilo Bernardo)

link:http://freecadweb.org/[FreeCAD]

IDF import for FreeCAD +
- Milos Koutny (milos.koutny@xxxxxxxxx)

link:https://github.com/jmwright/cadquery-freecad-module[CadQuery FC module] +
- CadQuery FreeCAD module +

link:https://bitbucket.org/hyOzd/freecad-macros[hyOzd freecad macros] +
- hyOzd parametric script

FreeCAD-PCB +
- marmni <marmni@xxxxxxx>

[[copyright]]
*Copyright*
-----------

This document '{docname}' is Copyright © 2015 by {Author}. You may distribute it and/or modify it under the terms of either
the GNU General Public License  (http://www.gnu.org/licenses/gpl.html),
version 3 or later, or the Creative Commons Attribution License
(http://creativecommons.org/licenses/by/3.0/), version 3.0 or later.

All trademarks within this guide belong to their legitimate owners.