cannot select the vertices for dimension and coincident constraints

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antondroid
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Joined: Tue Jun 14, 2022 11:48 am

cannot select the vertices for dimension and coincident constraints

Post by antondroid »

hi,
i had used freeCAD 0.20 few days, and all was fine, but at today i had find, that the points of the vertices cannot be selected for constraint dimension, and for coincident constraint with the arc.
i had find the few issues in internet, like this https://forum.freecadweb.org/viewtopic.php?t=29064
https://forum.freecadweb.org/viewtopic.php?t=26001
socket_wall_4_sq_new.FCStd
(978.53 KiB) Downloaded 11 times
but my points aren't every becomes green, it has keep red. But i can to select the lines, straight and arc.

the my real process is can be viewed by here https://youtu.be/m06_yYr8yZw

i had few time deleted the sketch itself, and even deleted plane, but the few attempts has the same result.

What can be happened with my freecad? may be i had accidentally some setting to denied the points selection or something else?

update:
after i had deleted the image planes (references), the vertices are becomes selectable .

so, i had supposed, that may be reference had fluenced to the vertices. (the reference planes was hide, while i drawing, i had open it, then hide, not constantly viewed.)

update 2: i had find now, that even if image planes are undeleted, it can be possible to select the vertices, but with very big zoom factor - about 40umx40um, but while it even 40mmx40mm, it i's impossible to select, instead of point, lines nearest can be selected.
[/code]
select_points.png
select_points.png (17.32 KiB) Viewed 822 times
but how to do if i want to use reference?

Code: Select all

OS: Windows 10 Version 2009
Word size of FreeCAD: 64-bit
Version: 0.20.29177 (Git)
Build type: Release
Branch: releases/FreeCAD-0-20
Hash: 68e337670e227889217652ddac593c93b5e8dc94
Python 3.8.10, Qt 5.15.2, Coin 4.0.1, Vtk 8.2.0, OCC 7.6.2
Locale: English/United States (en_US)
Installed mods: 
  * A2plus 0.4.56a
  * Assembly4 0.12.3
  * Help 1.0.3
  * lattice2 1.0.0
Last edited by antondroid on Wed Aug 10, 2022 1:46 pm, edited 2 times in total.
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Shalmeneser
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Re: cannot select the vertices for dimension and coincident constraints

Post by Shalmeneser »

The image should be 'below' the sketch.
Why are your pictures not at the exaact position ?

(btw, sketches : :shock: redondant dimensions or no constraints ?)
antondroid
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Re: cannot select the vertices for dimension and coincident constraints

Post by antondroid »

Shalmeneser wrote: Wed Aug 10, 2022 1:18 pm The image should be 'below' the sketch.
Why are your pictures not at the exaact position ?
of coarse, that are below, otherwise, how i can used these one while few days before.
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reference.png
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Roy_043
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Re: cannot select the vertices for dimension and coincident constraints

Post by Roy_043 »

In the file it is the other way around: Sketch loft_1s is below ImagePlane.
antondroid
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Re: cannot select the vertices for dimension and coincident constraints

Post by antondroid »

Roy_043 wrote: Wed Aug 10, 2022 4:56 pm In the file it is the other way around: Sketch loft_1s is below ImagePlane.
but what i need really to do? (even if i hide it visibility, the vertices didn't accessed)

what are you mean about 'below' in this case?

I had moved all reference planes behind the working plane, and i had move it constantly.

but if i will really modeling by the reference the complicate body, i think, that it must not have fluences to access to any point.

If to said about other CAD, i never meet with the case, that reference don't give access to the body vertices, while edges are still selectable.

i guess, may be this is bug or feature?
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Roy_043
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Re: cannot select the vertices for dimension and coincident constraints

Post by Roy_043 »

You have arranged the sketch below the image (sketch: Z=-1.6mm; image Z=0mm), and you are probably trying to edit the sketch from the 'bottom'. This does not work. In edit mode the points in the sketch are slightly raised to make selecting them easier, but this of course only works if you edit a sketch from the 'top'.

This has been discussed before, but I cannot find any previous topics ATM.
chrisb
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Re: cannot select the vertices for dimension and coincident constraints

Post by chrisb »

Roy_043 wrote: Wed Aug 10, 2022 9:54 pm This has been discussed before, but I cannot find any previous topics ATM.
Here is one: https://forum.freecadweb.org/viewtopic. ... 75#p616375.

@antondroid: Sketcher ViewSection can be very helpful if you have other objects before your sketch obstructing things there.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
antondroid
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Re: cannot select the vertices for dimension and coincident constraints

Post by antondroid »

Roy_043 wrote: Wed Aug 10, 2022 9:54 pm and you are probably trying to edit the sketch from the 'bottom'. This does not work. In edit mode the points in the sketch are slightly raised to make selecting them easier, but this of course only works if you edit a sketch from the 'top'.
so strange, if i need edit sketch namely from the bottom or from the rear, or any other side.

i think, this is bug, because in Inventor, for example, i can edit part, attached
to assembly from any direction, and it 's independent of the sketch level and direction.

i have moving the image plane every time now, it spend a much time, but this is fine for the simple modeling only.

i hope, that may be somebody would can fix it later.
Last edited by antondroid on Thu Aug 11, 2022 12:18 pm, edited 1 time in total.
drmacro
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Re: cannot select the vertices for dimension and coincident constraints

Post by drmacro »

antondroid wrote: Thu Aug 11, 2022 11:16 am ...
may be somebody can fix it later.
This has been a known behaviour of sketch editing for a long time.

"later" is a relative thing. ;)
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
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adrianinsaval
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Re: cannot select the vertices for dimension and coincident constraints

Post by adrianinsaval »

antondroid wrote: Thu Aug 11, 2022 11:16 am so strange, if i need edit sketch namely from the bottom or from the rear, or any other side.
Consider setting the MapReversed property of the sketch to true
i think, this is bug, because in Inventor, for example, i can edit part, attached
to assembly from any direction, and it 's independent of the sketch level and direction.
It's a known limitation rather than a bug, FreeCAD is not Inventor and has no relation to it so saying something works a certain way there is no basis for identifying a bug. That being said I believe this has been implemented in realthunder's fork so it's definitively possible to have that functionality in FreeCAD. I keep hope that these things will get merged eventually.
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