Projected Frontal Area from Assembly

[valhalla]

Greetings all,

I am using a Solidworks assembly that contains some lofted and rotated parts. Is there a way to project an outline of the assembly onto an offset plane and calculate the projected frontal area? A similar question would be for an umbrella. Is there a way to find the frontal area of the umbrella from an observers plane?
Thanks for the help.

 

[MadMango]

You should be able to create a new Plane, then select the model edges you want to see. Use the Convert Entities tool, and these edges should be projected on your Plane. Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[valhalla]

I had tried this. The prblem that I am having is that there are a lot of small edges in the projection angle and it takes time and a lot of zooming to select them all. We are trying to develop a tool that could be used in a concurrent design session (We'd love to find a command that we could macro if possible through the Solidworks API into Excel). The problem is similar to creating an orthographic projection in the drafting tools. Is there a way to create such a projection in a drawing file without having to manually select the surfaces to offset.

 

[MadMango]

I'm not aware of a Macro to do this.

You could save some time by selecting Faces instead of Edges. Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[DetroitPickles]

This may not help you, but may get everyone thinking.

If you know the furthest feature back from the "front", you could create a Section View (View : Display : Section View) along a parallel plane to the "front". Then select (click) the resulting "cut face", and get the Section Properties (Tools : Section Properties). The area will be listed of the face. If there are more than one flat faces, perhaps you have to add them up?

Ohh, well...
Mr. Pickles

 

[valhalla]

The section view and properties are close to what I want except that the part is rounded and hollow like an umbrella or bowl so I get the area of the face, but I need the area of the whole part. I tried building a mold part, cutting a cavity and selecting the cavity feature and clicking the convert entities, but I get the same error as just converting entities on the original object. Right now I am trying to use the Face Curves Tool on a 3D sketch, but this also seems to only allow me to pick one face on an object to convert. Maybe that will jog a few more ideas. Brian Lewis
The Aerospace Corporation

http://www.aero.org/

 

[DetroitPickles]

My mind isn't releasing anything new. I did discover how to get the minimum "box" size of your part. So in case you want to know how small of a box your part will fit into, I got that one figured out.

I did figure out that you can use the "Selection Filter". Set it to "Edges" and draw a box around your whole part. Then you could Control-Click on the edges you DON'T want included. Then do the Section Properties. But in your "cut a bowl in half" example, that isn't gonna work either...

It past my nap time...Can you make a drawing view of the face you want, and save it as a DXF and use AutoCAD's Area command on it? Oh my golly, did I use the dirty "A" word in here. Shoot me now folks, I'm a losing it...
Mr. Pickles

 

[SBaugh]

What about a RMB and click "select Tangency, loop, or Chain", depending on circumstances. Then you can convert your edges faster than selecting them all one by one while holding the control key down.

IHTH, Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.3dmca.com

faq731-376
When in doubt, always check the help

 

[TheTick]

How about this for a roundabout......

Make a single-view temporary drawing of the part, orienting the view to the plane you wish to project. Make sure this view is scaled 1:1. Export the drawing as *.dwg or *.dxf. Reimport into a SW part file, and you will have a 2D sketch of your projection. Gravity is a harsh mistress.

 

[valhalla]

Thats a pretty sneaky workaround. Is there a way to determine the overall area of the sketch though? I get a great 2D image, unfortunately, it also contains a lot of intermediate lines and SW won't extrude it until I clean it up. Takes as much or more time than selecting edges.

I tried selecting the loop to offset it and SW gives me an error that says Convert Entities Operation Failed.

I found another workaround in that if I created a block part the same height and width as my hollow part and used my part to create a cavity, the face that was left along with the area from a section view would give me the total area. I was just hoping to find a command that I could automate through VB into Excel rather than having to use these workarounds.

Thanks for the ideas though. Brian Lewis
The Aerospace Corporation

http://www.aero.org/

 

[TheTick]

Youo would still need to make some sort of feature out of it. My next step would be to either remove the inner curves or place another sketch on top of that and extract the outer curves. Then, make a planar surface feature and you can get the surface area. Gravity is a harsh mistress.