How to model a parametric hook?

[Christoph]

Hi,

maybe two years ago I tried to model a smooth looking parametric hook, but failed pretty much (because I couldn't find a way to place sketches on the right places). Now using Part Design next, the job can be done within 15 minutes. I like the new Part Design! The new tools like Datum Planes are a huge step forward for FreeCAD.

If you want to see how I designed the hook, follow the link to youtube (be aware, the video is in german):

Edit: I recorded the video again and tried to use your advices. Many thanks to you, I never ever saw a forum which is as helpful than this one!

phpBB [video]

[chrisb]

Nice video. In the first three minutes you don't need the construction lines. In 0.17 you can apply horizontal constraints directly to points. A serious problem can be the symmetry constraint. It might work - as it apparently does here - but it often leads to problems. Your Sketch is overconstrained because the symmetry implies the horizontal constraint.
More later, I'm short of time now.

[Kunda1]

Heads up: You can use the [video] tags to display videos
Nice job, btw.

[chrisb]

I have seen the rest and I am pleased by the usage of the datum planes as sections. I hope we will see more of your videos!
A final remark: The first datum plane is in fact the XY plane so you could omit it without any loss.

[tommeyers]

Christoph, Thanks for this tutorial. It came at the right time for me - a relatively new user. It am starting to put some of my jewelry designs in FreeCAD and will need to use those techniques. Tom Meyers

[freecad-heini-1]

Hi Christoph,
thank you very much, that is a nice video tutorial.

Please read this trick to avoid the many segments of the sweep-surface:
https://forum.freecadweb.org/viewtopic. ... 73#p180473

Concerning fillets, it's not needed to select so many edges if it's a tangent curve, one edge will do the job.
https://forum.freecadweb.org/viewtopic. ... 19#p198819

The helper sketcher lines are not needed, because there is another method to create the datum planes, please check my animation:

datum_plane_normal_zur_kante.gif (888.78 KiB) Viewed 1894 times

Please have a look at the zebra-tool inside the curves- and nurbs-workbench:
https://forum.freecadweb.org/viewtopic. ... 87#p204587

Best regards

Wilfried

[Christoph]

Hi,

thank you all for your feedback! Today I tried your advices, and the workflow is now much faster. Especially the orientation of the Datum Planes as advices from Wilfried lift the process up to a higher level. Only the conversion of the sweep sketch into a b-spline didn't work out, the sketch get always broken. Wilfried, do you have a solution for that?

I attach the file with the broken sweep sketch.

To avoid spreading working methods which are not ideal, I decided to record the video again (probably next weekend).

Regards
Christoph

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13532 (Git)
Build type: Release
Branch: master
Hash: 4adeb7702da610da2c7f3014217044167109f0d6
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: German/Germany (de_DE)

[freecad-heini-1]

Hi,

thank you all for your feedback! Today I tried your advices, and the workflow is now much faster. Especially the orientation of the Datum Planes as advices from Wilfried lift the process up to a higher level. Only the conversion of the sweep sketch into a b-spline didn't work out, the sketch get always broken. Wilfried, do you have a solution for

I'm glad that I could help you with the datum-planes.
Concerning the "convert given geometry to b-spline" tool, for me it seems that this tool is broken / has a bug.
I remember some cases with that tool in past, it worked like a charme.

But there is another great tool inside the curves workbench. It can convert a bunch of curves into one bspline curve.
Please let me show you a short demo:

join_curve_corner-break.gif (840.68 KiB) Viewed 1794 times

Please care about the data-tab, there is an option "corner-break", change into false.
Please try this trick on the crane hook for the sweep-profiles, and you will see a great result with a smooth surface.

Best regards
Wilfried

[freecad-heini-1]

@Christoph, please upload your freecad-file.

[freecad-heini-1]

Here you can see the difference.

1. conventional sweep:

conventional_sweep.png (82.77 KiB) Viewed 1740 times

fc017_sweep_normal.fcstd

(129.36 KiB) Downloaded 55 times

2. smooth sweep:

fc017_sweep_smooth.fcstd

(58.14 KiB) Downloaded 55 times

smoothl_sweep.png (75.78 KiB) Viewed 1740 times