Isoparametric TRIM/DIVIDE

[ravenzep]

Imagine a straight line that is revolved around the wcs origin... We get a cilinder. Easy enough. In revolve options, we set it to be a sheet body, and not a solid.
Now we apply the isoparam trim/divide..... well, it wont work.... it needs a face, and not a body. Fine.
Now we extract the face from that body, making the body invisible.
Now we invoke the command again, and we are now able to pick the face....But now comes the problem. It will only trim/divide along the non periodic direction.

So, how can i trim divide in the periodic direction.... or, how can i trim/ divide this shape in U and V as I please.

Thank you

 

[JohnRBaker]

What version of NX are you using?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[ravenzep]

Why is that so relevant?... The command has been around for some time i think...And is such a trivial operation anyway.

I am using NX 7.5, with the new update. As far as i know, the command is working pretty well. It clearly states it cannot be applied in the periodic direction, so i assume it s a restriction of the command, which is fair enough. I was looking for a solution rather than a comand bug... Command is working fine.

Thanks for replying.
Regards

 

[JohnRBaker]

Because if I, or someone else, found something which would accomplish what you needed we might want to offer you an example part file showing how it was done. Since you're running on NX 7.5 that won't be a problem, but if you were still back on say NX 5.0, someone might have wasted their time putting something together which you could never have been able to access.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[JohnRBaker]

While you can't 'Divide' in the periodic direction, you can 'Trim' it.

And if you would like a workflow which avoids having to extract a sheet body (at least at the start) try creating simple Isoparametric Curves on the face of the body and then use these to divide the face, which once that's done you can then use extract to get individual sheet bodies, if that was your final goal.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[ravenzep]

Hi John,
First of all thank you very much for being so kind and will to help in all your answers. Appreciated.
I understand perfectly what you are saying in your second answer. Would be easy to that on alias, on any place i wished, i.e. to place a isoparm, or to extract a isoparm at any precise location.

But NX is a diferent animal... is not so forgiving or so flexible, really. Different concept, which i love by the way. I thought about on how would i do that. Well, inserting isoparts through XFORM doesnt seem to be a solution to me. Through I-FORM, although it plants isoparms evenly spaced out doesnt seem flexible to place it where i want...neither a solution really... is used for other things. So i was left with curves from bodies menu... but neither of these are really isoparm insertion tools, i think.... intersecting the face with a plane (section) isnt really the same as extracting a isoparm, in concept anyway.

So, what would the best way to accomplish your solution? Seems like a good solution. How would i do that the best way in NX?

Thank you

 

[ravenzep]

Just thought of something simple that would solve it with trim/divide.... That is, to convert it to a non-periodic surface. For example rhino has this command.Can NX do something similar, or any trick to remove the non-periodicity? Remove parameters and making the body history free, will keep it periodic.
Then the trim/divide would work perfectly

Regards

 

[JohnRBaker]

I wasn't talking about X- or I-Form, bur rather simply...

Insert -> Curves from Bodies -> Extract -> Isoparametric Curves

...which can then be used to Trim the sheet body, as I did in the attached example.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[ravenzep]

YES, absolutely right you are. Can´t believe it was right under my eyes, and i skipped it. That s what using alias for too long lately does to you, i suppose. I was off NX for about 6 months, so i m getting back on track with it, as the the approach to solve surface challenges is totally different in NX.

And if i am allowed some moaning in the good sense, and some product feedback, i really ought to say that although catia (which i had to use) is a terrific application.... It died in time, if it was ever born (V5), it drived me nuts, and it s too old...PROe, is far too contraintful and wasnt my cup of tea really, not for surfacing with all the freedom I want.
So i see NX as the best of both worlds, and it did have a big evolution from the good old unigraphics. For a PLM software, it s the most flexible thing i have ever seen, and unlike many opinions, i do like the interface. Simply brilliant, at least for an engineer like myself.

Thank you very much for being so helpful, and thanks for having the time to send me a example file. Much appreciated. I really love this applicaton, extremely powerful and smart.

Best regards

 

[Toost]

You can not convert but yuo can "extract" from periodic to non-periodic, i.e the function you used , but maybe not saw the option in the bottom of the dialog :"Same as Original/ Polynomial Cubic / General B-surface".