NX6 - Revolve of closed curves

[ArchieH]

Hi,

So, here's a question that may not be NX-specific but I've not tried it on anything else so who knows!

If I wished to, for example, model a sphere I could sketch a semicircle and revolve 360 degrees about its diameter. Easy. However, logic would dictate that a circle revolved 180 degrees around its diameter would yield exactly the same result. NX, however, appears to be having none of it! Is anyone able to explain to my the reason behind this limitation?

I should note that I take no real issue with this, I'd just like to satisfy my curiosity!

Cheers guys,

 

[Toost]

Hm, I assume that you are not running 7.5.
I was pretty confident that i knew the answer on this one ( I have held quite a number of beginners classes over the years), then i tried it in 7.5 and noted that there has been a change.
You can in 7.5 revolve a full circle 180 and get an ok solid. Smaller angles give strange results though...
But in older releases, I think the following logic applies:
Assume that you instead of 180 degrees revolve the full circle any smaller angle, say 90 degrees, then you would have two resulting bodies, each 90 degrees, only connected at the center.
If the bodies were sheets, the connection would be point contacts, if the bodies would be solids a line-line contact, Both are more or less the foundation for the good old "non manifold body" message. Neither did older versions of NX "like" to produce multiple bodies per feature. So i assume that there were an if-statement somewhere in the code that prevented the case. See attached image.
Regards,
Tomas

 

[ArchieH]

As with most good answers, I now find myself wondering why I asked such as daft question! Thanks Toost. It does however highlight another curiosity, which is why does NX6 have such an issue with creating multiple bodies?

 

[Toost]

The old explanation on why "split body" previously killed ( removed parameters) was that one parameter could not work multiple bodies. This statement doesn't say anything on why but at least it's consistent... Maybe it is as simple as "the code has evolved and matured".

 

[JohnRBaker]

Is there an implication here that Revolving a full Circle 180° about an axis passing through the center of the circle will NOT produce a valid Solid body? UG/NX has been producing a VALID Solid using the scenario above since UG V18.0 (circa 2001). Granted, the resulting body is only HALF a sphere, but it IS a valid Solid. Now if you had revolved a full circle 360° about the axis, that would produced not only a valid Solid, but also a full sphere, even BEFORE UG V18.0.

Again, I'm not sure what you're implying with these questions about creating multiple bodies. UG/NX has always been able to create mutiple bodies from a single sketch. Granted, until NX 4.0, if the resulting Extrude/Revolve resulted in multiple bodies, there was a separate FEATURE created for each body but all the bodies whould still be valid (staring with NX 4.0, even though an Extrude/Revolve ended-up with more than one body, they would be considered to be part of the SAME feature).

If I've somehow misunderstood what the issues are here, please clarify what exactly it is that you're find odd or unexpected.

John R. Baker, P.E.
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Product Engineering Software
Siemens PLM Software Inc.
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[ArchieH]

Hi John,

Clearly I'm going to have to double check this tomorrow because, unless I've done something idiotic (and that's a distinct possibility! ) I'm pretty sure attempting to revolve a sphere 360° about its diameter produces an error in the version of NX6 we use.

As for my multiple bodies comment, I guess it sometimes appears to me that the 'cannot create multiple bodies' failure is not very uniform in its application. For example, I can make two bodies in a single extrude or by splitting a body but not by trimming a section out of one.

These are, by the way, questions arising from my own curiosity, and not, as I think you may have interpreted them, criticisms of NX.

 

[JohnRBaker]

In you comment above, when you say...

I'm pretty sure attempting to revolve a sphere 360° about its diameter produces an error in the version of NX6 we use.

...you really mean "revolve a circle", correct?

As for the splitting of a solid body into 2 parts by subtracting another solid, that depends on HOW and WHEN you did the Subtracting, or at least at one time it did.

Prior to NX 7.5, if you were creating a solid body that if it was subtracted from an existing solid it would split it into two parts, if you attempted this while you were actually creating the second body, it would fail. However, you could always just create the second body as a separate stand-alone body and then go back and perform an explicit Boolean Subtract and get the two bodies. Now up through NX 5.0 if you did this the result would be that all the parametrics would be removed from the first body and the no feature would be created, you'd just end-up with two unparameterized, or 'dumb bodies'. Starting in NX 6.0, despite the fact that you still couldn't perform the split operation during the creation of the second body, using the built-in Boolean, you could do it using an explicit Boolean subtract without losing any of your parameters or features and the resulting Boolean would stay a feature which could edited if you wished to. And as previously noted, starting with NX 7.5 the software doesn't care where you perform the Boolean, as part of the creation step for the second body or as an explicit Boolean, it now works no matter waht.




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.

 

[Toost]

Ok, hands up. I was wrong on the details.
But, ( the oldest version i have available is NX6.0) Try revolving the displayed example 0-180, then run an Examine Geometry - Select all.
I get Self intersecting face detected. ( The half sphere has 3 faces, two planar.)
Then try some other angles, ( Except 0, 180, 360) and have a look at the model.
The model in the attached picture is INVALID, to use the same vocabulary.
Regards,
Tomas

 

[JohnRBaker]

Note that I get what LOOKS like a valid model, which will, however, NOT pass the Examine Geometry tests (fails both Consistency and Self-Intersection). However, if you do a full 360° revolved body, it works just fine and passes all the tests with flying colors.

So perhaps it would be better to just do the 360° spin and then trim the sphere if the hemisphere was the final desired result. After all, if you created your circle using a Sketch, then you probably already have a Datum plane right where it needs to be for the Trim. Or just Sketch the closed semicircle and spin it 180°.

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.

 

[Toost]

John, this thread is from start a hypothetical discussion only. The recommended best practices ,"no geometry on the wrong side of the revolution axis", still apply.

Regards,
Tomas

 

[ArchieH]

Yup, I'm wrong too! Tried a 180 and 360 degree revolves of a full circle and got the hemisphere and sphere John said I would. I've no idea where I got the idea it hadn't worked in the past as I couldn't replicate the failure.

It's still interesting to note that a 360 degree revolve produces a sphere and a 180 a hemisphere. I would have expected the behaviour to be that a 180 degree revolve would create a full sphere and anything greater would produce a failure.

John, as Toost points out, this is purely hypothetical. I have no current need for a sphere, apart from anything else!

I'm grateful for your explanation on multiple bodies behaviour; it's always nice to know the expected behaviour and what to look forward to as and when we ever get around to upgrading.

 

[Toost]

John, This thread is really finished, but a last (?) clarification, when i said multiple bodies i meant multiple bodies, not features.
I.e currently NX allows a single feature to "manage" multiple bodies. In my perception ( -to safeguard my statement.. older versions of UG/NX did not allow a single feature to "manage" more than one body. As you noted an extrusion of a sketch consisting of "n" disconnected areas etc would produce "n" number of features/bodies but where feature/body always was 1/1.

 

[JohnRBaker]

Toost, yes, as can be deduced from my comments about the history of multiple body support in UG/NX, the concept of and the methods for creating them and their relationship to features, has evolved over time.

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.