Hi Maurice, The IDF export is wrong. If you can file a bug report with detailed instructions on how to reproduce the problem with the incorrect slot width that would be helpful. At the moment I can only reproduce the incorrect orientation of the slot.
- Cirilo On Sat, Jul 4, 2015 at 4:56 PM, easyw <[email protected]> wrote: > Hi Cirilo, > thanks for your feedback! > > to install the new freecad in debian I think it could be done with: > sudo add-apt-repository -y ppa:freecad-maintainers/freecad-stable > sudo apt-get update > sudo apt-get install freecad > (at least it worked for me in ubuntu where I had freecad 0.14) > > I have tried to export to IDF a board with a module with oval pads with > oval holes > I attached the board and IDF file > I seems that x and y are switched in the holes and the third hole also has > one incorrect diameter... > > could you please check if the problem is in the interpreting in freecad of > the file (I do not have solid works to check it) or if is a small bug in > the exporter? > > thank you very much again for you advices :) > Maurice > > > > On 04/07/2015 02.05, Cirilo Bernardo wrote: > >> 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 <[email protected]> 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 <[email protected] >>>> <mailto:[email protected]>> 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 : [email protected] >>>> <mailto:[email protected]> >>>> Unsubscribe : https://launchpad.net/~kicad-developers >>>> More help : https://help.launchpad.net/ListHelp >>>> >>>> >>>> >>>> >>
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
