Second Moment of Area: I-beam Assembly

[tomjk]

Could someone explain to me how I would find the second moment of area of an I-beam ASSEMBLY that is comprised of three rectangular prisms (2 for the flanges, 1 for the web)? I've been able to do it successfully when I created the I-beam as a single extruded solid with a continuous cross-sectional profile. I clicked Section Inertia... under Analysis, selected Existing Sections under Type, selected the whole cross-sectional profile, checked Second Moment of Area under Annotation, then chose Solid under Section Type in Settings. Now, with the assembly, I highlight the whole profile, keeping the other options the same, and I get a dialog box that says "Invalid data for Section Inertia Analysis"

 

[JohnRBaker]

What version of NX are you using?

John R. Baker, P.E.
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[tomjk]

NX 7.5

 

[JohnRBaker]

When you say 'ASSEMBLY' are we talking an actual 'assembly' where each segment of the 'I-beam' is a separate part file and what we see in your picture are 'Components' of the 'assembly'? Or are we simply talking about 3 separate extruded solid profiles which are modeled relative to each other but which still consist of THREE bodies in a single part file?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[tomjk]

John,

Thanks for your diligence in following up with my questions. To answer your question...it's the second choice. It's 3 extruded profiles that are modeled relative to each other and consist of three bodies. Sorry, I guess I shouldn't have called it an ASSEMBLY since it's not, by CAD definitions, an assembly. But I realized the problem NX was having with my profile was there were three separate enclosed rectangles so maybe it was trying to take the second moment of area of each one separately or something...?

Anyway, I've actually figured it out how get the second moment of area value I wanted. It was a bit tedious, but I knew what had to be done was to create a profile of the perimeter of the I-beam, and I accomplished that through exporting it as a parasolid, uniting the bodies then Insert -> Curve from Bodies -> Section and this created the perimeter like profile I needed for the Section Inertia analysis.

But what I do need to ask you is, since this process was a little long-winded:

Is there a way to create a section view (to expose the cross-section of a part), easily create a profile sketch of the perimeter, in other words have the program trace a profile around the edges of the part that are exposed as a result of the section view, and then from there I can run a Section Inertia analysis using that new cross-sectional profile? See this was just a simple example I set up to figure out how to get the area moment of inertia value in NX, but in reality, I need to find the area moment of inertia of a complicated "acutal" assembly.

 

[JohnRBaker]

Why not just Unite the 3 bodies?

But if for some reason you don't want to do that, you can do what I did in the attached example. Using the Offset Curve function with the Offset = 0.00, I used the Curve Selection tools to select 'Single Curves' with the 'Stop at Intersection' option toggled ON and walked around the profile of the 3 'assembled' solids until I had a 'profile' which I then used to perform the section analysis.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[tomjk]

John,

Where do I find the Single Curve with Stop at Intersection option in the Curve Selection tool, after I start the Offset Curve function?

 

[JohnRBaker]

You toggle ON the icon on the Selection Bar, as shown below:

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Walterke]

Using the Offset Curve function with the Offset = 0.00,

Is there a difference between this and using project curve?

If it were me I'd just create a new sketch, project the curves and do the calculation there.

Also: I'm assuming the "stop at intersection" button is an advanced modeling tool? Because I can't find it either.

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[JohnRBaker]

It's NOT an 'advanced modeling' option.

These extra couple of icons will appear or are active ONLY when their use would be relevant based on either the function that you're performing OR the 'Curve Rule' that you've chosen. For example, if you select 'Face Edges' these 'Stop at Intersection' and 'Follow Filet' options are irrelevant and so remain inactive. Sometimes, when the function being performed could never be able to use either of these options, then the icons will not even be shown, inactive or otherwise.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[tomjk]

John,

Thanks for all of your help. I am satisfied with your approach