Extrude up to "offset surface"?

[CNSZU]

Hi all,

In solidworks (see attached image) you can extrude a cylinder and specify the end condition to be offset a certain dimension (eg 5 mm) from a specified surface (surface A). Is there a similar way to do the same thing in NX? All I can think of is you need to first create a plane which is offset 5 mm from surface A, then you choose the end condition "until selected" in the extrude tool and choose the plane. This is more troublesome and creates extra clutter in the part navigator. Please advice.

 

[mmauldin]

For that particular model, you could extrude to a distance. For the distance value select "Fomula", in the expressions pop-up select "measure" and then measure the length of the loongest vertical edge and add 5mm to that result. The result will be associative. See attached.

This may be less effective for more complicated models.

 

[jerry1423]

Check into "replace face" in "syncronous modeling". You can specify an offset in that. It is very handy !

 

[mmauldin]

Another option would be to place the sketch on the reference surface and just use a simple value. See attached.

 

[JohnRBaker]

And if you make the sketch internal, you'll have even less "clutter in the Part Navigator".

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[CNSZU]

For the distance value select "Fomula", in the expressions pop-up select "measure" and then measure the length of the loongest vertical edge and add 5mm to that result. The result will be associative.

This is a good method, but I would suggest to measure distance from the sketch plane to the end surface instead of an edge because it's closer to the design intent.

One small problem with this method is that it's hard to figure out how the cylinder is modeled because the formula is not highlighted in the model. You need to go into the Expressions dialog box, then select the "length27" measurement, then click the Measure Distance icon to find out what "length27" means.

Check into "replace face" in "syncronous modeling". You can specify an offset in that. It is very handy !

Could you create a part to show how this is done for this model?

Another option would be to place the sketch on the reference surface and just use a simple value.

This is the easiest way, but it is preferable to sketch on the original datum plane to comply with correct modeling practices.

So, for now I think using a formula is the best way, but I would like to add the following footnote: NX is lacking in the ability to "direct edit" dimensions. It is sometimes a pain to have to navigate through a myriad of dialog boxes to make adjustments.

 

[JohnRBaker]

What version of NX are you running? If it's at least NX 7.5, have you ever tried using...

Edit -> Feature -> Edit Dimension...

...where you simply select the feature you wish to edit and the dimensions will be presented in a list for you to edit.

Alternatively you can also do something similar using the Part Navigator (and this has been working way before NX 7.5). Just select a feature in the list, expand the 'Details' panel at bottom of the Navigator and you'll see the parameters (dimensions) of the feature listed. All you have to do is double-click the parameter that you wish to edit, make the changes and hit return and the model will update. No need to "navigate through a myriad of dialog boxes to make adjustments".

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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