links to objects go out of allowed scopes + Cut not working as expected

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Qubix
Posts: 2
Joined: Mon Mar 20, 2023 3:44 pm

links to objects go out of allowed scopes + Cut not working as expected

Post by Qubix »

Hi everyone, I am following this tutorial by jokoengineeringhelp step-by-step. He shows how to make a header/manifold: https://www.youtube.com/watch?v=gT4nfh1u6LA

Just like in the video I made the sketches and pad in Partdesign. When I applied the extrusions on “sketch001” and “sketch002” through Part workbench the following messages appeared in the Report view:
Part::Extrusion: Link(s) to object(s) 'Sketch001' go out of the allowed scope 'Extrude'. Instead, the linked object(s) reside within 'Body'.
20:16:59 Part::Extrusion: Link(s) to object(s) 'Sketch002' go out of the allowed scope 'Extrude001'. Instead, the linked object(s) reside within 'Body'.
In the dependency graph there are red arrows pointing from the extrusions to the sketches. What does all this mean?

At 9:50 He applies an cut between “extrude” and extrude001”. However, when I try to do the same thing no cut appears. Instead “extrude001” dissappears without anything changing on “extrude”.
Does this have anything to do with my previous question? How do get it to work like in the video?

Code: Select all

OS: Windows 7 Version 6.1 (Build 7601: SP 1)
Word size of FreeCAD: 64-bit
Version: 0.20.2.29177 +426 (Git)
Build type: Release
Branch: (HEAD detached from 0.20.2)
Hash: 930dd9a76203a3260b1e6256c70c1c3cad8c5cb8
Python 3.8.10, Qt 5.15.2, Coin 4.0.1, Vtk 8.2.0, OCC 7.6.3
Locale: Dutch/Netherlands (nl_NL)
Installed mods: 
  * A2plus 0.4.60k
  * CurvedShapes 1.0.4
  * Curves 0.6.8
  * fasteners 0.4.55
  * freecad.gears 1.0.0
  * sheetmetal 0.2.61
Attachments
Manifold dependency graph.png
Manifold dependency graph.png (36.73 KiB) Viewed 671 times
Manifold.FCStd
(21.64 KiB) Downloaded 13 times
chrisb
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Re: links to objects go out of allowed scopes + Cut not working as expected

Post by chrisb »

Hi and welcome to the forum!

I hope you don't expect every helper here to watch a 45 minutes video? It looks to me that something went wrong either in the video or in your understanding of it.

A PartDesign body is is a small universe with limited interaction with the outside world. Using something from inside in a Part tool is forbidden, you should use Pads instead of extrudes in that case.
A Body is always a single solid, the features are not standalone objects, every followup feature includes all its predesessors. So you should not derive things to bool from a single body, use additive and subtractive features inside of the body instead.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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papyblaise
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Re: links to objects go out of allowed scopes + Cut not working as expected

Post by papyblaise »

t's a very very difficult exercise even for a youngster like me who started 25 years ago :lol:
I looked for a long time why it didn't work, I found an insestuous relationship between the origin of the 2 curves and the Pad in the body which makes the cut impossible
I have not read the video, you never know which version they refer to and often the author makes fantastical operations :!:
Attachments
manifold.JPG
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manifold PPB.FCStd
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edwilliams16
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Re: links to objects go out of allowed scopes + Cut not working as expected

Post by edwilliams16 »

If you want to use the same sketch both inside and outside a Part Design Body without getting "Out of Scope" errors, you can use a PartDesign SubShapeBinder. In your case, make binders of the two sketches and drag them outside the body. You can then Extrude or do whatever with them in the Part Workbench.

It's slightly simpler the other way around. Create your sketches with the sketcher outside the body and then create binders of them inside the body. You can pick and choose the elements of the sketch you intend to use. This is one realization of the Master Sketch workflow.

Here's an example:
Screenshot 2023-03-21 at 7.42.34 AM.png
Screenshot 2023-03-21 at 7.42.34 AM.png (37.15 KiB) Viewed 570 times
Screenshot 2023-03-21 at 7.44.01 AM.png
Screenshot 2023-03-21 at 7.44.01 AM.png (16.84 KiB) Viewed 570 times
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PDSubshapes.FCStd
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Qubix
Posts: 2
Joined: Mon Mar 20, 2023 3:44 pm

Re: links to objects go out of allowed scopes + Cut not working as expected

Post by Qubix »

Thanks everyone for your responses.
chrisb wrote: Tue Mar 21, 2023 1:43 pm I hope you don't expect every helper here to watch a 45 minutes video?
I certainly don't expect that. I just posted the link and timestamp because I thought it would make it easier for others to understand what I am trying to do.
edwilliams16 wrote: Tue Mar 21, 2023 5:47 pm If you want to use the same sketch both inside and outside a Part Design Body without getting "Out of Scope" errors, you can use a PartDesign SubShapeBinder. In your case, make binders of the two sketches and drag them outside the body. You can then Extrude or do whatever with them in the Part Workbench.
Thanks! This has helped me get rid of the red arrows in the dependency graph and the "Out of Scope" errors messages.
I am still trying to get the cut to work exactly like in the video. I guess I just need to look more into how cuts and other boolean operations work.
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