(SOLVED) How to draw a nipple?

[NormandC]

That's nice renato, but your sweep produces a self-intersecting shape that may cause problems with boolean operations. I'm quite surprised that you were able to cut it from the cylinder with no apparent errors.

FC_self-intersecting_sweep_01.png (41.54 KiB) Viewed 1549 times

You need to reduce the height of the triangle profile in Sketch002 so half its height is less than the helix pitch. Then you are sure the sweep is not self-intersecting:

FC_non-intersecting_sweep_01.png (14.62 KiB) Viewed 1549 times

Also, you should not rely on dimensional constraints so much. You should use geometric constraints where possible. See Sketch002 in my revised file.

[AvgJoe]

I just wanted to recrate the model to learn it. Unfortunatly the current "stable" freecad realase cannot cut out the thread correctly. The latest(?):
Word size of FreeCAD: 32-bit
Realease date 26/01/2015/
Version: 0.15.4531 (Git)
Branch: master
Hash: 8628a6e0e0ef9223bff722b1278e5211039ae1b7
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1
cannot create a helix without braking the shape. Than the cut option even doesn't come up when it should. (The attached file was made with the stable version.)

[jmaustpc]

I just wanted to recrate the model to learn it. Unfortunatly the current "stable" freecad realase cannot cut out the thread correctly. The latest(?):
Word size of FreeCAD: 32-bit
Realease date 26/01/2015/
Version: 0.15.4531 (Git)
Branch: master
Hash: 8628a6e0e0ef9223bff722b1278e5211039ae1b7
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1
cannot create a helix without braking the shape. Than the cut option even doesn't come up when it should. (The attached file was made with the stable version.)

I have had a quick look at your last file....it will not work the way you tried to make it.

Read what Norm and others have posted regarding this topic.

You have a
1) the sweep along the helix is self intersecting
2) the outer face of the sweep is co-planar with the outer face of the cylinder "PadTubeOD".
3) the helix uses the same diameter as the cylinder which can sometimes lead to problems, particularly with some FreeCAD OCE version combinations.


If you are modelling this because you just want to learn how to model something and know little about CAD (nothing wrong with that) ....then I suggest you start with less complex items and progress step by step.

Jim

[AvgJoe]

I modified the drawing as you suggested but the result was the same. ("same" file)

I couldn't find out what am I doing wrong.
But I was able to create a nipple with following this tutorial:
http://www.metalshaperman.com/?p=2009
...and drilling a hole into the cylinder.

Thank you all for your kind help and time!!!

[jmaustpc]

Hi
Your sweep still contains self intersections.

If you go to the Part WB ...Part menu...check geometry ....but you have to turn on extended BOP checks to find this particular error in this case. By default the extended BOP checks are not enabled.

I think the problem is that your sweep path...the helix...is outside the sweep profile. Decrease the diameter of the helix so that it is inside the resultant sweep and I think your problems will go away.

I think this is only a problem in some versions of OCC/OCE (the CAD kernel used by FreeCAD), so you may get different results with different FreeCAD versions and also depending on which libs your FreeCAD was compiled against.

Jim

[bejant]

For me the helix seems to be broken into several individual 360* turns instead of one continuous helix, so when I create a Sweep it only travels one revolution around the helix:

20150131a-OneTurnHelix.png (12.72 KiB) Viewed 1425 times

When I create a new helix, it appears the same way.
Does anyone else experience this, or is it just me?

OS: Ubuntu 14.04.1 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.15.4532 (Git)
Branch: master
Hash: dc623f264660b9a671d73d17dee824e002796a0d
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1

[quick61]

Hi bejant,

I think that is the current working fix for long helix heights. After so many turns, or certain height, can't remember which, the helix would fail. Double clicking the helix selects all the segments.

Mark

[NormandC]

I believe it's the result of a workaround for a helix bug.

See comments in issue #954

[mario52]

hi

It seems that every height between 194 and 225 will cause problem other values are ok

here Helix problem
and here 0954 Workaround for Helix Primitive
mario

[bejant]

First, thanks for the help!

I couldn't find out what am I doing wrong.

I think the problem is that your sweep path...the helix...is outside the sweep profile. Decrease the diameter of the helix so that it is inside the resultant sweep and I think your problems will go away.

I changed the helix radius to 41.30016 mm, the Sweep and a subsequent Cut work and Check Geometry reports no errors. But the threads end abruptly at the top and bottom:

20150131b-AvgJoe.png (27.02 KiB) Viewed 1403 times

So AvgJoe may want to move the helix down Z = 3.17 mm and change the helix height to 41.27 mm.