Ticket #4498 - Loft and two pads, non-manifold, can't fillet edges?

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robotarmy
Posts: 11
Joined: Fri May 31, 2019 2:43 am

Ticket #4498 - Loft and two pads, non-manifold, can't fillet edges?

Postby robotarmy » Tue Nov 17, 2020 1:30 am

Hi all,

Really excited to be using this for my day-to-day MCAD package, but I can't figure a way around this issue:

I'd like to join two tangent cylinders, with different diameters, using a lofted section. I've made two sketches on two planes offset from each other and lofted between them, then used the sketches to create pads from either side of the loft.

The sketch that defines the 'profile' of the loft operation is properly connected to the pad adjacent ('sketch' in the attached file). The other end of the loft, (defined by 'sketch001' in the attached) doesn't seem to attach properly to the pad adjacent. When I export the STL and open it in Cura, it complains and shows me the rendering in the attached screenshot.

I'm also unable to fillet either edge between the lofted section and the pads.

I tried to make a new sketch with the same two circles as would be in 'sketch001', and pad using that, and it failed in the same way.

I've also tried to make a new sketch with unrelated geometry (a circle of random diameter) and attach it to the same face at the wide mouth of the loft, and it won't do an 'additive' pad, only a 'subtractive' one, cutting into the body.

Have I found bugs?

OS: macOS 10.15
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.22756 (Git)
Build type: Release
Branch: master
Hash: ce87f586ee36ffe8ebcdcd3947ced4ab389ae795
Python version: 3.8.6
Qt version: 5.12.5
Coin version: 4.0.0
OCC version: 7.4.0
Locale: C/Default (C)
Attachments
Screenshot 2020-11-16 at 17.18.39.png
Screenshot 2020-11-16 at 17.18.39.png (677.97 KiB) Viewed 324 times
vacuumadapter.FCStd
(126.15 KiB) Downloaded 8 times
Last edited by Kunda1 on Sat Nov 21, 2020 5:15 pm, edited 1 time in total.
Reason: Added ticket number to thread title
zardozer
Posts: 8
Joined: Sat Nov 07, 2020 2:35 am

Re: Loft and two pads, non-manifold, can't fillet edges?

Postby zardozer » Tue Nov 17, 2020 7:22 am

I looked at your loft, and I think I see the issue. If you look at the wireframe, it's trying to map the inner part of one circle to the outer part of the other:
Wireframe.png
Wireframe.png (75.78 KiB) Viewed 299 times
So the larger circles at the bottom have their wall reversed, and when you try to pad that, it gets confused.

If you go to your sketches, you'll see that when you created your circles, it numbers the circles edge1 for the first outer circle, then edge2 for the second inner circle in the order they were created. But when you created the second pair of circles, you reversed the order in which you created the circles so the outer is 2 and the inner is 1. I believe when you loft, it tries to match the edges in order. You'll be able to see this in your loft when you mouse over the sections, it's kind of split into two. Not sure if this is considered an "invalid" loft, but it did let you make it.

To fix this, you'll have to go into one of the sketches and delete one of the circles, and make sure the order matches. Then you'll be able to pad either side properly.
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papyblaise
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Location: France

Re: Loft and two pads, non-manifold, can't fillet edges?

Postby papyblaise » Tue Nov 17, 2020 7:26 am

your Loft is crossed: the sketches are not drawn in the same order: if in the first you draw the inner circle, then the outside, in the 2nd skecht you must respect the same order
I can make a thread on the exterior angles, if I try on the interior angles it crashes
I don't know why, but a chamfer works
Attachments
manifold.FCStd
(223.77 KiB) Downloaded 6 times
manifold.PNG
manifold.PNG (15.51 KiB) Viewed 297 times
chrisb
Posts: 29062
Joined: Tue Mar 17, 2015 9:14 am

Re: Loft and two pads, non-manifold, can't fillet edges?

Postby chrisb » Tue Nov 17, 2020 8:43 am

I have added this issue to the Limitations section of PartDesign AdditiveLoft. Please validate if it is correct and clear.
A Sketcher Lecture with in-depth information is available in English, auf deutsch, en français, en español.
robotarmy
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Joined: Fri May 31, 2019 2:43 am

Re: Loft and two pads, non-manifold, can't fillet edges?

Postby robotarmy » Thu Nov 19, 2020 4:41 am

That's brilliant! Thanks for the response all.

The limitation text in the wiki is clear and sensible.

Should this be filed as a bug/improvement request somewhere? Seems like it's something that could be checked for and corrected programmatically, at least for simple shapes?

Awesome!
chrisb
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Re: Loft and two pads, non-manifold, can't fillet edges?

Postby chrisb » Thu Nov 19, 2020 7:36 am

robotarmy wrote:
Thu Nov 19, 2020 4:41 am
Should this be filed as a bug/improvement request somewhere? Seems like it's something that could be checked for and corrected programmatically, at least for simple shapes?
I think it could indeed be distinguished between inner and outer loops, thus this makes a sensible request in the bug tracker. Check if there already exists a ticket in the PartDesign section. If not, please create a ticket with a link to this discussion. Classify it as a feature request. And add a link here to reference back to the ticket. You can use the "bug" button to create the tags where you only have to put the number in between.
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robotarmy
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Re: Loft and two pads, non-manifold, can't fillet edges?

Postby robotarmy » Sat Nov 21, 2020 6:43 am

chrisb
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Re: Loft and two pads, non-manifold, can't fillet edges?

Postby chrisb » Sat Nov 21, 2020 7:41 am

robotarmy wrote:
Sat Nov 21, 2020 6:43 am
Like this? issue #4498
Yes!
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Kunda1
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Re: Loft and two pads, non-manifold, can't fillet edges?

Postby Kunda1 » Sat Nov 21, 2020 4:41 pm

robotarmy wrote:
Sat Nov 21, 2020 6:43 am
issue #4498
@chrisb do you think this should get addressed in the 0.19 release or bump to 0.20 ?
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chrisb
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Re: Ticket #4498 - Loft and two pads, non-manifold, can't fillet edges?

Postby chrisb » Sat Nov 21, 2020 5:48 pm

It could well be moved, because it is no regression. It may even be classified as a feature request.
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