creating a point at the center of an area

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

snipped-for-privacy@gmail.com wrote:

Get the section into DWGEditor. Use the REGION command to make a region of the entities that define the section. (A region is like a 2d solid. No, not a surface!) Then use the MASSPROP command to get all sorts of info on the section.

I thought I remembered seeing a tool for this in SW somewhere, but I can't find it now.

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

"Wayne Tiffany" wrote in news: snipped-for-privacy@roc.usenetexchange.com:

You're right. I did miss the point. Section modulus is just I/y, so it can easily be calculated by hand if you know where the neutral axis is. Of course, that may not be trivial... Come to think of it, the MASSPROP command won't give it either because the bend direction isn't specified. This needs a macro, I suppose.

I don't have time for either macro. How often does this center of area need to be dealt with? Often enough to be worth the trouble? Otherwise I recommend what Dan suggested, but using copy & paste with Notepad, instead of writing things down.

On the other hand, ModelDocExtension::GetSectionProperties2 looks like a very straightforward method. Perhaps it wouldn't be too hard to modify the CG macro, if the OP can't find any volunteers, this might be a good opportunity to get his feet wet with macros. Modifying an existing macro is easier than starting from scratch.

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

Good one. It's easy to forget about reference points.

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???

Create another sketch on that same face containing a point coincident to the reference point. Show the sketch it you drawing view, and the point will be visible.

I just noticed that you can import these into the drawing using Import Model Items.

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