Extrude to vertex or point.

[cobaltred]

Win 7 64 NX 8.5 Is there a way to extrude to a vertex or point in NX for the end condition.In Solidworks you can extrude to vertex which I have used often.

Thanks, Buddy.

 

[kukelyk]

A point/vertex cannot limit an extrusion, it need a direction too, so You need a plane through the vertex.
Or you can make an associative measure parameter :distance of the vertex from the plane of the profile, and use this as end value of extrude.
You should define an UDF for this.

----
kukelyk

 

[SvenBom]

When you create a body with Extrude command, click with Right Mouse Button on an end arrow of the extrude. In the list, you will have Snap to Object. Select a point somewhere on a body, and extrude will be created up to this point. But beware, this is not an associative connection. If the selected points move, the extrude (that used this point in Snap to Object) will not move.
Attahced is the movie of how this is working (If this is what you have been looking for).

 

[cobaltred]

Thanks, the avi movie explains. So you can do it but it is not associative, Wouldn't it be easier if NX simply added up to point to the end condition choices? and is there any reason why it could not be associative.
And to the first answer, yes I am fully aware that an extrude needs a direction, I was just talking about the end condition and the fact that many other cad packages have up to point as a choice.

Thanks Buddy

 

[JohnRBaker]

A 'point' IS a choice, when using 'Snap to Object', just that it's not associative. If you think it should be associative, please contact GTAC and they will be more than happy to help you open an ER (Enhancement Request) covering this topic.

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.

 

[SiW979]

Or use the measure command from within side the extrude function, measure from the start to the point and you will have an associative extrude.

Cheers

Si

Best regards

Simon NX 7.5.4.4 MP8 and NX 8.5 (native) - TC 8

http://www.jcb.com

 

[cobaltred]

Very good, I have tried all the suggestions and I can live perfectly happy that. Thanks.

 

[aluminum2]

I saw your post and wondered the same exact thing with the extrude command. Why can't I just select a point like in solidworks. I am aware of the measure workaround, but it still is not as quick. I submitted an ER and hopefully Siemens will add it on a later release.