CAD Forum

Posted: **Wed Apr 07, 2021 12:24 pm**

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

Thx

Mark

Posted: **Wed Apr 07, 2021 12:33 pm**

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.

Posted: **Wed Apr 07, 2021 12:39 pm**

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.

Posted: **Wed Apr 07, 2021 12:45 pm**

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!!

Posted: **Wed Apr 07, 2021 12:56 pm**

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

Posted: **Wed Apr 07, 2021 1:15 pm**

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

Posted: **Wed Apr 07, 2021 1:18 pm**

mbiasotti wrote: ↑Wed Apr 07, 2021 12:24 pm 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

Posted: **Wed Apr 07, 2021 1:28 pm**

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

Posted: **Wed Apr 07, 2021 1:32 pm**

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.

Posted: **Wed Apr 07, 2021 1:34 pm**

jcapriotti wrote: ↑Wed Apr 07, 2021 1:18 pm
mbiasotti wrote: ↑Wed Apr 07, 2021 12:24 pm 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.

Posted: **Wed Apr 07, 2021 1:34 pm**

@Jaylin Hochstetler

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

Posted: **Wed Apr 07, 2021 1:35 pm**

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

Posted: **Wed Apr 07, 2021 1:36 pm**

Roasted By John wrote: ↑Wed Apr 07, 2021 1:34 pm @Jaylin Hochstetler

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

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

Posted: **Wed Apr 07, 2021 1:39 pm**

matt wrote: ↑Wed Apr 07, 2021 1:35 pm 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.

Posted: **Wed Apr 07, 2021 1:59 pm**

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

Posted: **Thu Apr 08, 2021 8:47 am**

mbiasotti wrote: ↑Wed Apr 07, 2021 12:24 pm 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.

Posted: **Thu Apr 08, 2021 9:38 am**

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

Posted: **Thu Apr 08, 2021 9:49 am**

@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 ..

Posted: **Thu Apr 08, 2021 10:33 am**

mbiasotti wrote: ↑Thu Apr 08, 2021 9:38 am 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.

Posted: **Thu Apr 08, 2021 10:39 am**

dpihlaja wrote: ↑Thu Apr 08, 2021 10:33 am
mbiasotti wrote: ↑Thu Apr 08, 2021 9:38 am 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.

Posted: **Thu Apr 08, 2021 10:58 am**

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

Posted: **Thu Apr 08, 2021 6:23 pm**

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.

Posted: **Thu Apr 08, 2021 8:24 pm**

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

Posted: **Fri Apr 09, 2021 7:28 am**

zxys001 wrote: ↑Thu Apr 08, 2021 8:24 pm ..four equal lines, 2 collinear and 2 perpendicular with the endpoints on the surface. (image/file)

Ding Ding, Winner Chicken Dinner

Posted: **Fri Apr 09, 2021 8:14 am**

mbiasotti wrote: ↑Thu Apr 08, 2021 6:23 pm 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?

Posted: **Fri Apr 09, 2021 8:54 am**

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

Posted: **Fri Apr 09, 2021 9:03 pm**

@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:

Posted: **Mon Apr 12, 2021 8:09 am**

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

Posted: **Wed Apr 21, 2021 12:30 pm**

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

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How to place point at the center of a sphere?

How to place point at the center of a sphere?

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