[v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane. [solved with 2 sweeps][bug 1739]

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industromatic
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[v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane. [solved with 2 sweeps][bug 1739]

Post by industromatic »

I have a body containing a flat topped cone and pad located to an origin that is numbered 004, but has no translations from origin 1.
I copied a sketch for my additive sweep and reworked it to be what needs to be trimmed to keep some drafted bosses bottom edges from sticking out when put in a corner. When I sweep it, I get some of the cone left there:
cs-enc-spread-driven-6-subtract-1.png
cs-enc-spread-driven-6-subtract-1.png (27.17 KiB) Viewed 1821 times
cs-enc-spread-driven-6-subtract-2.png
cs-enc-spread-driven-6-subtract-2.png (27.72 KiB) Viewed 1821 times
cs-enc-spread-driven-6-subtract-3.png
cs-enc-spread-driven-6-subtract-3.png (38.56 KiB) Viewed 1821 times
cs-enc-spread-driven-6-subtract-4.png
cs-enc-spread-driven-6-subtract-4.png (44.33 KiB) Viewed 1821 times
cs-enc-spread-driven-6.fcstd
(211.93 KiB) Downloaded 22 times
  • OS: Debian GNU/Linux testing (buster)
    Word size of OS: 64-bit
    Word size of FreeCAD: 64-bit
    Version: 0.17.11967 (Git)
    Build type: Release
    Branch: master
    Hash: d0c5865f323aa9555662912f2ff96188f29096a6
    Python version: 2.7.13
    Qt version: 4.8.7
    Coin version: 4.0.0a
    OCC version: 7.1.0
    Locale: English/UnitedStates (en_US)
Last edited by industromatic on Fri Sep 08, 2017 3:40 pm, edited 3 times in total.
peterl94
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane.

Post by peterl94 »

It looks to be the same problem as is in this thread: https://www.forum.freecadweb.org/viewto ... =3&t=24230.

Would you be willing to upload your file? It's easiest to troubleshoot that way.
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industromatic
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane.

Post by industromatic »

File is now attached to first post next to the screenshots.

If this is due to non-overlap of the path start and stop, how do I answer the PartDesign subtractive pipe dialog so there is an overlap.
It says, select sections to sweep, and it is not possible to select any of them twice to overlap.
Last edited by industromatic on Fri Sep 08, 2017 4:14 am, edited 1 time in total.
peterl94
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane.

Post by peterl94 »

Actually, it is not what I thought. I think you have run into a known bug with subtractive sweep. It doesn't currently work with closed loops. In your case you may be able create a separate non-loop sweep to cut each corner.
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sweep-loop-error.FCStd
(27.63 KiB) Downloaded 24 times
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industromatic
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane.

Post by industromatic »

create a separate non-loop sweep to cut each corner.
So, go into the additive pipe dialog twice, each time for overlapping sections?

OK, tried that. I swept counter clockwise from start, then CW from start, overlapping the first sweep sections, and no sliver.

Here is the file again in case you see anything else non-recommended to point out.

I am all ears, wanting to get a real enclosure to mill out soon.
cs-enc-spread-driven-7.fcstd
(226.68 KiB) Downloaded 24 times
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industromatic
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane. [solved with 2 sweeps][bug 1729]

Post by industromatic »

I reported this as matching bug 1729 https://www.freecadweb.org/tracker/view.php?id=1739

But it could be more as the ragged shell visible in the first 3 render screenshots above is not just at the end of the sweep, but along the side wall also for a random amount of area. Are there any other known bugs like that?
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane. [solved with 2 sweeps][bug 1739]

Post by peterl94 »

I believe the problem is caused by the sweep not being united with itself, and not a tolerance issue as reported in the issue you linked. In fact, I'm not sure if anyone has created a ticket for this issue yet.

For example, the end face shown in the preview should not be there.
sweep1.png
sweep1.png (43.4 KiB) Viewed 1698 times


It works if the face is not over anything being cut, but completely fails, if the sweep is making a cut all of the way around, like in the file I posted.
sweep2.png
sweep2.png (61.39 KiB) Viewed 1698 times
industromatic wrote: Fri Sep 08, 2017 1:20 am Here is the file again in case you see anything else non-recommended to point out.
You may have to introduce some shape binders into the mix now that the cross coordinate system link prevention has been merged. This is what ickby said about it, if you are wondering the reasoning behind the restrictions.
The restrictions on links is kind of a feature. It creates some boundaries to what you can do, however, with this we ensure that all freecad document objects works like the user expects them to. So not a feature in a sense of new things, but a feature n the sense of keeping things working and logical.
It is generally now required to create a shape binder when you need to reference geometry in a different part or body. The shape binder will then correctly handle the different coordinate systems.

I find your construction method a bit odd, but not knowing your design intent, I can't really say if there is a better way. I mean I see box with radiused corners, a lip, and a couple studs, but I don't know what the most important parameters are and how much they should be able to be modified.

Thanks for sticking with it! I'm sure learning FreeCAD can be a frustrating experience, but the issues you find help make FreeCAD better.
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industromatic
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Re: [v0.17] Subtractive pipe leaves some bits not subtracted at start/stop plane. [solved with 2 sweeps][bug 1739]

Post by industromatic »

ShapeBinders are in a different topic than this, so I'll talk about them under a new heading.
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