Reason of error

[cubalibre000]

Hi,
I'm not looking for a solution, but only understand the reason of this error.
As you can see, the Extrude(6) fail.
Why the 'until next' is not aceptated by NX, in this case ?
How NX ratiocinates with this option enabled ?


Thank you...

Using NX 8 and TC9.1

 

[cowski]

In this case, "until next" is accepted and it did work; you get an alert, not an error.

The issue is: no new material is added to the solid in this case.

The defining curves are coplanar with the top surface and the "until next" option uses the side and bottom faces to trim your new extrude. "Until next" looks at all the faces your new extrude interacts with, not just the bottom cap face.

www.nxjournaling.com

 

[cubalibre000]

Thanks for the answer, but as you write, why no new material is added ?
Sorry but SolidWorks and Solid Edge in this case add material and Parasolid is the same engine.

Thank you...

Using NX 8 and TC9.1

 

[cowski]

...the "until next" option uses the side and bottom faces to trim your new extrude.

If you change the boolean option to "none" you will see what the extrude command has created.

I was answering in context of how NX works, which I thought was what the original question was asking. Personally, I don't often use the "until..." options as they are prone to update errors. I think they can be improved upon and possibly combined. If you'd like to see a change/improvement, your best option is to contact GTAC with an IR/ER.

www.nxjournaling.com

 

[Toost]

This has nothing to do with Parasolid. Parasolid does NOT have Features, Features such as Extrude is a part of the implementation of Parasolid in the cadsystem. Also the rules and options which the specific cad system provides is in the "implementation" , not Parasolid. Therefore Extrude, as an example, has different options depending on the cad system. Assume that you as the Cad system developer would like to implement a new feature, "Revolve with twist" , then Parasolid must provide a such option to create this type of geometry, but you as developer must "wrap" the option into a usable feature, with dialog options, editability etc etc. Parasolid only "delivers" the geometry.

In NX the option "Until Next", the "target face" for the extrusion must be large enough to cover the Full area of the extrusion. If not one must use the "Until extended" which will extend the target face. Probably this is implemented differently in SE and SW.

Regards,
Tomas