NX6 - Revolve of closed curves
NX6 - Revolve of closed curves
(OP)
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,
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,





RE: NX6 - Revolve of closed curves
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
RE: NX6 - Revolve of closed curves
RE: NX6 - Revolve of closed curves
RE: NX6 - Revolve of closed curves
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.
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.
RE: NX6 - Revolve of closed curves
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.
RE: NX6 - Revolve of closed curves
...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.
RE: NX6 - Revolve of closed curves
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
RE: NX6 - Revolve of closed curves
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.
RE: NX6 - Revolve of closed curves
Regards,
Tomas
RE: NX6 - Revolve of closed curves
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.
RE: NX6 - Revolve of closed curves
I.e currently NX allows a single feature to "manage" multiple bodies. In my perception ( -to safeguard my statement..
RE: NX6 - Revolve of closed curves
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.