To be able to use this reference to create a plane in an assembly
A small addition to better understand. I would like to replace the spheres so that they have a reference in their center so that I can make a plane like the red arrow in my drawing and create a clip for the connected ones
avavec_dimensions.jpg
A sketch will do the trick, for example:
- If it is to create the sphere, a boss per revolution of a line is a semicircle, so the center of the sphere will be the midpoint of the line,
- If the sphere exists, a 3d sketch of a right triangle whose vertices are tengeant to the sphere, so the center will be the midpoint of the hypotenuse. It also seems to me that a constraint of concentrecity with a point is also feasible!
Good evening
You can very well put a constraint between two points, each state in different parts possibly.
Which version of SW do you have?? Because there are new possibilities with the 2019 and especially the 2020 and 2021.
Kind regards
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Hello
I have the 2015 version, can I apply a constraint between two points with this version?
Good evening
If the sphere was created with SolidWorks, it was probably based on a sketch with an arc of a circle whose center is the center of the sphere. Just make the sketch visible to access this point later.
If the sphere has been imported and does not have a sketch for its generation: simply measure the diameter of the sphere, then build a 3D sketch with a simple segment and a point in the middle. The ends of this segment are constrained to be on the spherical surface, and the distance from the midpoint to one end of the segment is dimensioned with the value of the radius. The segment in question is then a diameter of the sphere, its midpoint being the center.
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Thank you for your answer, but could you send me a diamond sphere. 10 and a point in its center, I'm not sure of your solutions, I can't reproduce it.
A small sphere file by webtransfer would be nice.
Hello@tous
Attached is a description of my previous comments, I specify that the concentric point center does not work (I was wrong)
doc2-2.pdf
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Hello
@fauteux1959: Unfortunately, I don't have a version of SolidWorks compatible with the 2015...
The principle of the last @Lynk proposal seems to me to be the most effective: to construct two segments carried by two spokes. The center is at the intersection of these segments.
The attached video offers a simplified version of this principle, which avoids the construction of the two tangent planes.
centre_sphere.mp4
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Hello
I find that the two tangent planes remain the solution for those who don't master geometry too much.
foreground
second
and the median plane on which a sketch is drawn, which is the intersection of the plane and the sphere
Or another solution
plane tg plus perpendicular segment whose end is attached to the surface of the sphere
The center of this segment is the center of the sphere
Sorry for the duplicates.
Hello
To solve this problem, I trusted the possibilities of Solidworks in sketches
This gives the center of a sphere in 3 parallel planes and a simple sketch on the middle plane
The Part file is in SW 2021
Kind regards
centre_dune_sphere_-_3_plans_paralleles_et_une_esquisse_simple_.jpg
centre_dune_sphere_-_3_plans_paralleles_et_une_esquisse.sldprt
Hello
If it's a nice sphere, why not create a point with the reference geometry tools?
Simply select the surface and request the point in the center of the face.
Impossible to open your file future version me I sw 2015
Hello@Frédéric
Excellent solution except that for the requester it is not a perfect sphere but a sphere with a cylindrical tail.
Can you tell us how you would do in this case. It's always interesting to see how colleagues solve problems.
Kind regards
@Fauteux1959
If my ultra-simple method suits you, can I make you an animated gif or a video?
I put a short film where I present the way to create a shot with three references, I managed to create the first two references, the center of the two spheres. But the third I don't know what to put the final plane would be inclined through the center of two spheres
https://www.youtube.com/watch?v=foWlw1ufLs8&list=PL-BB6m5xrUdNWCjpWrnxp-8E-DWl9Szrf
3rd ref is the center of the sphere at the bottom left for example
It all depends on the position of the plane you are looking for.
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Hi all
Here is another solution to recover the center of a spherical, or partially spherical, element.
The advantage of this solution is that it does not use tangency (in a sketch or between faces) which tend to be capricious.
-1 copy the spherical surface with " Surface-Offset "
-2 Transform the copied surface which is a portion of a sphere into a complete sphere with " Surface restore "
-3 Create a " Point " (Reference Geometry -> Point) with the option "Center of the surface".
Kind regards.
centre_de_sphere.jpg
centre_de_sphere.sldprt
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