Measure Bodies vs. Area using Curves

[ablad]

Hello,

I am trying to create a C# program that finds the centroid of a face and I have a few questions about the different centroid calculating tools in NX 7.5.5.

Why are my centroid measurements different when I use the Measure Body command versus when I use the area using curves command? (For measure body I extruded an intersection curve equally in both directions, for area using curves I measured with the cross-sectional face of the object at the same height as the intersection curve. I also compared with the area using curves of the intersection curve itself.)

When using the Area using Curves command, why would different centroids be found when using a face versus a curve (section or intersection)?

Is there any way to utilize the area using curves command in NXOpen and C#?

Which tool is most accurate for finding the centroid of a face?

Thank you.

 

[kapmnit123]

Hi,
How much difference in values are you getting? Ideally both of them give the same value.Though i will prefer to use MEASURE BODIES if you already have a solid to run the analysis on.
One probable reason i can think of why your results are not matching is that AREA USING CURVES results depend on the WCS orientation .
Here are some excerpts from NX documentation for AREA USING CURVES.
"Calculates and displays geometric properties of planar figures. This function analyzes figures after projecting them onto the XC-YC plane (the work plane). True lengths, areas, etc., are obtained by changing the WCS so that the work plane is parallel to the plane of the figure."Hope that helps.
Best Regards
Kapil Sharma

 

[ablad]

Hi,

When I compare the analysis of curves command for the face of my body and an intersection (or section) curve at the same point my delta is 0.0004 inches in the X and 0.0003 inches in the Y.

Comparing the analysis of curves of an intersection curve to the measure body of an extruded intersection curve, I am getting deltas of 0.002 inches in the X and 0.0005 inches in the Y.

My WCS is set to absolute, so I don't think that should have an effect.

Thanks

 

[cowski]

Have you tried changing the tolerance in the measure using curves command?

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[ablad]

Yes I have. I use a tolerance of 0.0001 when using the analysis using curves command. If I use a larger tolerance (ex. 0.01) the values are more similar to those of the measure body command. Is there a way to increase the tolerances when using measure bodies?

 

[aluminum2]

I wonder if it could be the tolerance of your constructed features and curves. I know when I extrude or revolve a sketch, my tolerance default is .001.

 

[Toost]

If I was you I would try to stay away from the area using curves....
It has a number of rules that one needs to know and follow if one wants a correct answer from it.
As mentioned, it will project the selected curves onto the XC-YC and measure the area inside the projection.

Now the tricky part, It uses the same "boundary" definition as NXCAM part does (did?) when selecting the curves, and unless you know how that works, ....
- The curves must be selected in order,
- The curves must be selected having the same "direction", (all clockwise or all counterclockwise)
- Holes must have a opposite direction else the hole area will be added. ( select the arc on the correct spot to get the correct direction)
- When selecting holes one must press "new boundary" else the hole will be connected to the outer boundary.
If you want to try i recommend the Permanent Boundary option, where the resulting boundary is visible and one can see ones mistakes.

But, it does report a number which is "identical" to the area using faces if one manages the boundary definition
See attached image for a correct boundary. ( if the hole / outer is clockwise or counter clockwise doesn't matter as long as they are opposite.)

Regards,
Tomas

 

[JohnRBaker]

For one thing, the 'Area Using Curves' method is a legacy function from when NX (only it was UG back then) did not yet include support for Solid Models (the 'style' of the dialogs should have given you a hint as to its age).

Now if all you have is a planar set of curves to define your profile, be it a sketch or just a closed set of curves, try using...

Analysis -> Section Inertia...

...and see if this gives you what you're looking for.

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.

 

[ablad]

That helps a lot.

Thank you to everyone for the help!!

 

[ablad]

I actually have one more question. Should I expect a difference in centroid between the Section Inertia and the Measure bodies? I am seeing a difference in centroid between using the Section Inertia with an intersection curve vs. Measure Bodies with an extrude made from that same intersection curve.

 

[cowski]

Is the difference within your set modeling tolerance?
If so, I wouldn't worry about it.

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[JohnRBaker]

In the simple tests that I've performed, the centroids were consistent.

Could you provide a sample where you're getting this discrepancy? Or if you can't supply the actual part file could you at least provide a picture of what the profile looks like? Also, are you working in Metric or Imperial units?

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.

 

[kapmnit123]

Hi,
Could you please send us a picture of the intersection curve you are trying.
Best Regards
Kapil Sharma

 

[kapmnit123]

Hi,
Please check if the settings for SECTION TYPE is SOLID (for section inertia)
Best Regards
Kapil Sharma

 

[ablad]

The intersection curve I am working with looks similar to the outside edge of a NIKE swoosh, but a bit flatter. I am using Imperial units and I did use a solid section type for the section inertia analysis. I am seeing deltas of about 0.003 inches between the section inertia and measure bodies. The same intersection curve is used for the section inertia and to create an extrude for the measure bodies command, which is what is really confusing me in terms of the measurement differences. When the curve is created, a tolerance of 0.0001 is used.

The model came to me already built, so I don't want to mess with the modeling tolerances if possible.

Thanks

 

[cowski]

As long as the difference you are seeing is much less than the size of your model, I wouldn't worry about it.

Measure body uses an accuracy tolerance of 0.99 by default (I see no way to change that in the dialog); it is an iterative calculation. What this means is, NX "chops up" the body it is measuring into easy to calculate chunks (for illustration we'll say they are cubes for a volume calculation). It then adds up the chunks to get the total answer. It then cuts the model up into smaller cubes and does the calculation again. It repeats this until the current answer is less than 1% different than the previous iteration. The answer given is a very close approximation of the true value; what you are seeing is most likely the differences in the calculation approximations.

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