Sketcher broken face
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- Posts: 52
- Joined: Tue Dec 28, 2021 12:24 pm
Sketcher broken face
I have this fully constrained yet I get this error.
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +99 (Git)
Build type: Release
Branch: Branch_0.19.3
Hash: 6530e364184ce05ccff39501e175cf2237e6ee4b
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United States (en_US)
OS: Windows 10 Version 2009Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +99 (Git)
Build type: Release
Branch: Branch_0.19.3
Hash: 6530e364184ce05ccff39501e175cf2237e6ee4b
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United States (en_US)
- Attachments
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- clamp2.FCStd
- (22.1 KiB) Downloaded 17 times
Re: Sketcher broken face
Did you use Validate sketch to see if there are issues?
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
Re: Sketcher broken face
Fully constrained doesn't mean well constrained.
Your sketch isn't closed. There is at least one missing coincidence at the top right.
EDIT : also why are you using "Internal alignment" constraints ?
Your sketch isn't closed. There is at least one missing coincidence at the top right.
EDIT : also why are you using "Internal alignment" constraints ?
Last edited by openBrain on Mon Jan 17, 2022 3:00 pm, edited 1 time in total.
Re: Sketcher broken face
Which is because the solver is not a algebrical one but iterative (not sure if this is the correct terminology). So while matematically two points should be at the same place in reality they might not be. A little exagregated example but two vertical dimensions stacked on top of each other might fall within the desired tolerance (say +-0.1mm) but if they are both have +0.09mm error their sum will be with +0.18mm error which is more than the desired +-0.1mm. That way if the two verticas should be coincident they might not become such. In such cases if they should be coincident specifically indicating so by using coincident, point on point tangency, point on point perpendicularity, will ensure it.
I edited a little your first sketch to reflect that.
I edited a little your first sketch to reflect that.
- Attachments
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- clamp2_kiss.FCStd
- (29.04 KiB) Downloaded 12 times
Re: Sketcher broken face
This problem is almost certainly caused by the use of "grid snap". In FreeCAD it is very dangerous because it can appear that there are proper connections when there are not.
If a connection is wanted, as in this case, one should explicitly create it by Coincident, Tangent, or one of the other appropriate constraints. Autoconstraints will also work in many cases, if used correctly.
Snapping two elements to the same grid point will *not* work.
Gene
If a connection is wanted, as in this case, one should explicitly create it by Coincident, Tangent, or one of the other appropriate constraints. Autoconstraints will also work in many cases, if used correctly.
Snapping two elements to the same grid point will *not* work.
Gene
Re: Sketcher broken face
I think it is good to think of a coincident constraint as a property of two end vertexes.
Their physical proximity (which is achieved with grid snap) does not indicate coincidence.
It is in fact possible to have a constrained sketch with no coincident vertexes that will Pad successfully. But, this requires a very well thought out constraint scheme. Thus for most mere mortal users, it will be best to specifically define coincident vertexes.
As noted, the term fully constrained does not imply well constrained. And, there are other solver behaviours (like large changes in spreadsheet driven dimensions causing the shape to change in unexpected ways) that take some experience to tame.
Their physical proximity (which is achieved with grid snap) does not indicate coincidence.
It is in fact possible to have a constrained sketch with no coincident vertexes that will Pad successfully. But, this requires a very well thought out constraint scheme. Thus for most mere mortal users, it will be best to specifically define coincident vertexes.
As noted, the term fully constrained does not imply well constrained. And, there are other solver behaviours (like large changes in spreadsheet driven dimensions causing the shape to change in unexpected ways) that take some experience to tame.
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
Re: Sketcher broken face
Not sure of this. Here it looks like actual coincidence/smooth joint is achieved by induced constraining through dimensional constraints, which is not good at all.
Re: Sketcher broken face
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- Posts: 52
- Joined: Tue Dec 28, 2021 12:24 pm
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- Posts: 52
- Joined: Tue Dec 28, 2021 12:24 pm
Re: Sketcher broken face
I don't know why I clicked that or what it does. Though I watch tutorials and read the Wiki, there's still a little try this when something isn't working.