creating a point at the center of an area

I can use the properties to locate the center of area, but how do I
creat a point in that location.
For example: create a point in the center of area of a triangle.
Thank you

 

I use the section data to locate the point. Take a section, write down
the coordinates, and then create a sketch using thoses coordinates.
This will work until you change the geometry and the center moves. I'd
love another way, and maybe there is one.

Also, my company often asks for section modulii which solidworks
doesn't compute (I have to use ProE to calculate this, and I hear about
it from the ProE guys). I'd love to have this integrated also.

Dan Sommerfeld
Industrial Designer
ITW Dahti Technologies

 

Aren't you guys sort of missing the point? The OP said that he could read
the coordinates by using the Tools/Section Properties tool. But then how
does he put a point there? Manually typing those numbers into a 3D sketch
is a way that would work. But, I would think that those numbers would be
available to the API, so I think what he wants is a macro just like the one
we have for putting a 3D point at the CG. There are 2 macros that do that -
one that puts a new point every time you run it, and the other that updates
the one existing point. Both are static in that they don't automatically
update. So, someone with some time could take the CG macro and rewrite it
to a Center of Area macro. I don't have the time right now - any takers up
to the challenge?

WT

 

You can add a "Reference Point" to the "Center of Face" on any shape
surface...

Insert/Reference Geometry/Point

This is the same tool used for inserting a plane or an axis. See
Reference Geometry.

This is not to be confused with...

Tools/Sketch Entities/Point

 

Ahhh, touche. I don't believe I have ever used that one, but I think it
hits the nail in the head here as the best solution without a macro. If you
add the point and then modify the shape of the face, then the point will not
move on its own. However, if you then edit the definition of that reference
point, it will update properly. You can use that point to attach lines,
etc. (Don't forget to turn on the viewing of points.)

That's why I like this group - thanks.

WT

 

if you are looking for a way to generate a point at the center of mass,
which is what it kinda sounds like, there was a post about a week ago
that had a macro that would generate a point at the center... hope
that helps...

Jeff

 

FYI - I sketched a triangle and extruded it. I then inserted the
reference point. Click on the point and record the coordinates. If you
then go back to the triangle sketch and drag one of the vertexes and
leave the sketch the reference point has moved to the new centroid of
the area. (SW2006SP2)
~G

 

Now that is interesting. The way I tested it was by changing the shape by
double-clicking to show a dimension, change the dim, then rebuild. The
model and the face updated, but the point did not. But if you go into the
sketch to make the change, the point will update when you come out. You
don't have to rebuild to come out, just close the sketch. So, two different
methods - I wonder if SW knows about this??

WT

 

Wayne, I tried your method too and all updated, even the point. It is
now in a different location. Strange ... it works both ways for me and
I cannot recreate your scenerio.

I contribute this to Bermuda Triangle Surface rather than Boolean
Triangle Surface.... goof luck!!

Its snowing like crazy here so I think I am going to cut out.

Have a nice weekend.

~G

 

Thank you all for he helpful information.

The "Tools/Sketch Entities/Point" command work great for faces.

What I have been trying to find is a way to creat a point in the COG of
a chained 2d object witout going into DWG editor. It would be nice to
be able to create the point while in sketch mode but the above command
will work for what I need.

I use this to determine the center of effort in relation to the center
of lateral resistence in sailboat design.

Thanks,
Randle

 

I have yet to find a way to create a point at COB in drawing mode.
If I do the "Tools/Sketch Entities/Point" command in PART mode the
point it works good, but will not show in DRAWING mode.
hmm......
any ideas???

 

Chub,

To get this point to show in drawing mode ...

In part mode right click on the point in the design tree and select
Show.
Then in drawing mode View\Points

~G