NX 7.5 Diameter dimesion in revolved sketch 1

[ErickF]

Hello guys.

I'm new in NX and need some help to get my designs better in it.

I'm trying to create a diameter dimension (diameter value) when I do a revolve feature using the center line (reference line) as shown in the attached image.

I used to do that in a simply way in ProE by clicking in the point (line end), in the center line and in the point again, but I can't do something like this in NX.

Is it possible to do that or the only way is to put the value divided by 2?

Thanks!

 

[cowski]

You can mirror your OD line about the center line and convert it to reference; now you will be able to place a driving dimension that controls the OD.

www.nxjournaling.com

 

[ErickF]

It worked, but also increased the complexity and clicks in sketch.

Thank You anyway!


Pro Engineer user trying to understand NX.

 

[JohnRBaker]

Alternatively, create a user-defined Expression representing the desired Diameter, and then when you model the sketch which will be revolved, simply dimension the one half using the formula 'sketch expresion = Diameter/2'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[ErickF]

Thank You so much guys.

Now I realized that is not possible to do it in a "natural" way in NX. But no problem. I'll get used to it.

Pro Engineer user trying to understand NX.

 

[JohnRBaker]

The issue is that despite what you might think, while creating a Sketch there is no real way for the system to know 100% how that sketch will eventually be used. What I mean is that you might start out thinking that the sketch you're creating will only be used for a revolved section, but once completed there's nothing stopping you from using that same skerch to also create an extrude.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[ErickF]

Thanks again, John.

I understand what you mean.
My idea is to use this dimension in the drawing whit the "Feature Parameter", thats why I want to put the "final" dimension.
At least I think the Feature Parameter is the tool to take de model dimension in the drawing.

If there is another way or another tool to do that, please tell me.
I don't want to compare NX to ProE all the time, but there I use the command "Show/Erase" to bring the sketch dimensions to the drawing "automatically".

Sorry for the basic questions.

Pro Engineer user trying to understand NX.

 

[JohnRBaker]

Of course, once the part is created, a PMI reference diameter dimension could be added to the model which could then be inherited onto your Drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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