How to place point at the center of a sphere?

[mbiasotti]

Does anyone have a good method of placing a 3Dsketch point or Ref point at the center of a spherical body?

Thx

Mark

[MJuric]

Depends on how the Sphere was created.

If it's a revolved half circle with a sketch, then show the sketch and place the point on the midpoint of the line.

Otherwise you have to create planes, axis and then intersect the axis with the remaining plane.

[Roasted By John]

If you can't do what @MJuric mentioned then you could add six tangent planes and draw four lines equally spaced using the planes to anchor the line end points.

[Arthur NY]

Possibly two construction lines set up on axis with the points at the ends of the construction line made to have an "on surface" relationship. Then where they cross you can place the point. It's a workaround at best....but there really should be a way to grab this already in the software.

Along with grabbing the center of an object (i.e. tube) that can get the path that is at the center of the geometry. Have been wanting this forever!!

[AlexLachance]

Isn't there a sort of temporary axys created by spheres? I don't really work with them which is why I'm asking

[matt]

This will probably depend on the kind of data you have, but if it is a real sphere you can use Face Curves and work it from there.

image.png

[jcapriotti]

Does anyone have a good method of placing a 3Dsketch point or Ref point at the center of a spherical body?

Reference Geometry/Point worked for me

image.png

[matt]

You can also use a 3D sketch to draw a line, make it touch the sphere on one end, then make it perpendicular, then make it touch the sphere on the other end, and then make a midpoint.

Older versions of SW do not let you sketch a point at the midpoint of a line, but they fixed that at some point.

image.png

[Jaylin Hochstetler]

I made a sphere via a revolve on the Front Plane (which like @Roasted By John said, you could put your ref point on the center point of that line or if you would use a midpoint line it would make it automatically) After that I made a sketch using the Right Plane which was in the center of the sphere then I made 2 construction lines that the end points were coincident to the quadrants on the outside of the sphere. Like this:

2021-04-07 13_12_09-Window.jpg

Then I dropped a point on the intersection
which resulted in this:

2021-04-07 13_31_09-Window.jpg

Don't know if this is any help, but thought I would give my 2 cents.

[MJuric]

Does anyone have a good method of placing a 3Dsketch point or Ref point at the center of a spherical body?

Reference Geometry/Point worked for me

image.png

Well I mean if you want to do it the easy way...you could do that

I have never tried that and never even though to think of a sphere as a spherical face.

[Roasted By John]

@Jaylin Hochstetler

You need to adjust your 2 cents for inflation, for the most value

[matt]

Oh, I like this game we should play this one more often.

- From a random view, RMB on sphere and select "Create Plane Normal To View"
- open a sketch on new plane
- select silhouette edge of sphere
- convert entities
- exit sketch
- create axis normal to plane through center of converted edge
- rotate view randomly
- RMB on sphere and select "Create Plane Normal To View"
- open sketch on new plane
- select silhouette edge of sphere
- convert entities
- exit sketch
- create axis normal to plane through center of converted edge
- open 3d sketch and place a point, make it coincident to both new axis features.

image.png

[Jaylin Hochstetler]

@Jaylin Hochstetler

You need to adjust your 2 cents for inflation, for the most value

Mine don't inflate--backed by pure gold.

[jcapriotti]

Oh, I like this game we should play this one more often.

- From a random view, RMB on sphere and select "Create Plane Normal To View"
- open a sketch on new plane
- select silhouette edge of sphere
- convert entities
- exit sketch
- create axis normal to plane through center of converted edge
- rotate view randomly
- RMB on sphere and select "Create Plane Normal To View"
- open sketch on new plane
- select silhouette edge of sphere
- convert entities
- exit sketch
- create axis normal to plane through center of converted edge
- open 3d sketch and place a point, make it coincident to both new axis features.

Matt, you win for most complicated way to add a point to the center of a sphere.

[matt]

Oh, oh, oh, call on me please!! One more, one more.

Use Center Of Mass (assuming it's the only solid body in a part)

image.png

[DanPihlaja]

Does anyone have a good method of placing a 3Dsketch point or Ref point at the center of a spherical body?

Thx

Mark

image.png

Just use reference point and "Center of Face"

Does it automatically. Assuming it is actually radial.

[mbiasotti]

Thanks for all of your thoughtful replies -I'm still studying them. The assumption for my issue is that this is an import and I don't have access to the base feature that created the sphere. Also, the spherical face of the model is partial.

If the Spherical face was a full face, then the best I've found is to use the Reference point feature with the option of "Center of face" which puts the ref point exactly as the center (as Jason and Dan have suggested). So the process for me is to get the face back to a full sphere using Delete Hole or delete face. If neither of those work then the exercise becomes a bit harder. Here is the example of the part, a human mannequin and this is just one limb - and others were equally challenging:

Femor-right.sldprt

(3.35 MiB) Downloaded 163 times

[Roasted By John]

@mbiasotti

I added a perpendicular line to your 3DSketch2

Then I added Plane2

Then I added Cut-Extrude1 - to cut the part in the center of the two spheres

Now you can add whatever you need for a reference, then mirror bodies ..

[DanPihlaja]

Thanks for all of your thoughtful replies -I'm still studying them. The assumption for my issue is that this is an import and I don't have access to the base feature that created the sphere. Also, the spherical face of the model is partial.

If the Spherical face was a full face, then the best I've found is to use the Reference point feature with the option of "Center of face" which puts the ref point exactly as the center (as Jason and Dan have suggested). So the process for me is to get the face back to a full sphere using Delete Hole or delete face. If neither of those work then the exercise becomes a bit harder. Here is the example of the part, a human mannequin and this is just one limb - and others were equally challenging:



Femor-right.sldprt

What about untrim? If it is indeed a spherical face, then untrim should work to bring it back to a full sphere.

[DanPihlaja]

Thanks for all of your thoughtful replies -I'm still studying them. The assumption for my issue is that this is an import and I don't have access to the base feature that created the sphere. Also, the spherical face of the model is partial.

If the Spherical face was a full face, then the best I've found is to use the Reference point feature with the option of "Center of face" which puts the ref point exactly as the center (as Jason and Dan have suggested). So the process for me is to get the face back to a full sphere using Delete Hole or delete face. If neither of those work then the exercise becomes a bit harder. Here is the example of the part, a human mannequin and this is just one limb - and others were equally challenging:



Femor-right.sldprt

What about untrim? If it is indeed a spherical face, then untrim should work to bring it back to a full sphere.

Yup, untrim works well.
See GIF below.

[jcapriotti]

@dpihlaja Nice....untrim is amazing at times.

[mbiasotti]

Yes - untrim also as a method of getting back to full sphere. I believe I use untrimmed in the model I posted. If not I did use it on this model attached. It didn't get back to a full untrimmed sphere but did get me far enough to get a useable reference.

[zxys001]

..four equal lines, 2 collinear and 2 perpendicular with the endpoints on the surface. (image/file)

[Roasted By John]

..four equal lines, 2 collinear and 2 perpendicular with the endpoints on the surface. (image/file)

Ding Ding, Winner Chicken Dinner

[DanPihlaja]

Yes - untrim also as a method of getting back to full sphere. I believe I use untrimmed in the model I posted. If not I did use it on this model attached. It didn't get back to a full untrimmed sphere but did get me far enough to get a useable reference.

All you had to do was run the untrim command twice, which gave you a full sphere.

Yeah, 100% isn't predictable for this. If the old forum were still alive, here is where I would link one of my own questions on the forum: What does 100% untrim really mean?

[Rob]

Here's an idea

Pop your part into an assembly.

Create a virtual part and float it, before mating it concentric to the sphere face.

Then edit the part in context and create a point using point on point to the origin of the virtual part.

If you don't want an external ref, you could use a 3d sketch point instead.

Unfortunately if you break refs, the point feature fails, but the sketch is happy.

To work entirely without ex refs, (and the part is not going to change) just fix a sketch point.

You can then delete the assembly.

this could be very quick if you have lots of spheres to work with as you can just edit the mate and capture the origin with a fixed sketch point

[mbiasotti]

@dpihlaja Hi Dan, great point - although I was actually referring to the first model I posted (Femor-right.sldprt) where the furthest I could take it was this:

[elmarklammer]

Hello Marc,

I would create a plane that intersects the sphere at any given distance. Create the 3D sketch as shown in the image using equal distance constraints and you will have your center point.

Elmar

[Krzysztof Szpakowski]

Use 3D sketch - 2 lines with a common one end
Add relations: Ends lines on surface and line perpendicular to surface for both.
Its all
Common end is at center