Dimensioning cylinder after edge blend

[ForrestAnderson]

I am having some issues with a dimension on a draft. The person that I would normally ask this question is going to be out of contact for quite a while.

Attached are some photos of the draft, that I will be refering to. I am going to have a spool that I have designed machined. The flange before the edge blend is applied is 3" in diameter, and I want to show that on my draft. As you can see in a previous draft the correct diameter was dimensioned, but I have no idea how it was done. Looking at the dimension associativity the two angles that form the flange are selected on both sides, but I have no idea how that was done.


Thanks in advance.

 

[PSI-CAD]

Hi,

What NX version are you using ?


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[ForrestAnderson]

NX 8

 

[PSI-CAD]

Hi,

Find herewith an example

1°) Create a sketch on the view
2°) Project the top curve (arc) that becomes a line
3°) Place the cylindrical dimension with intersection point selection

I hope this help


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

They probably created a pair of 'Intersection Symbols' by going to...

Insert -> Annotation -> Intersection Symbol...

...created the dimension and then hid the symbols:

John R. Baker, P.E.
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[ewh]

That is what I would have done (without hiding the symbols of course).

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[jerry1423]

yes but when you use the intersection symbol you cannot use the cylindrical dimension, which includes the diameter symbol.
It's just a little but of a hassle to add the diameter symbol in appended text.

Maybe an enhancment in NX could include the ability to add a cylindrical dimension to these two points after the direction of the cylinder is specified.

 

[JohnRBaker]

Actually there's a way to get EXACTLY what you want without having to do anything special. Just create your Cylindrical Dimension between 'Snap Points' using the 'Two-curve Intersection' method, as shown below:

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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UG/NX Museum:

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

 

[PSI-CAD]

As ForrestAnderson is in NX8, the sketch is necessary because 'Two-curve Intersection' method doesn't work until NX8.5.

Could you confirm John ?


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[ewh]

Which takes longer, creating the sketch or adding appended text? What is the true difference when it comes to interpreting the drawing?

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[JohnRBaker]

It's fully supported in NX 8.0. In fact, it's been supported since NX 2.0, released nearly 10 years ago.

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.

 

[PSI-CAD]

Hi John,

I suppose that you answer to me. I didn't say that the function is not supported, but it does'nt work with this geometry. And I have found that it works in NX8.5

Please open my part and try in NX8 to place the dimension at 'Two-curve Intersection' after deleting the sketch in view. NX doesn't find the intersection without any message !!!


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

You're comparing 'Apples and Oranges'. The example ForrestAnderson provided was adding this Dimension to a Section View, which has been doable for nearly 10 years. My two examples were also done in the context of a Section View. In Sections Views you have real 'curves' which can be referenced just as if you had manually drawn them yourself.

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.

 

[PSI-CAD]

Hi John

Do not be sarcastic with me. I enjoy this forum because I find a lot of solution and I try to give also my contribution.

I apologize for my mistake but by this way I found a limitation:

In NX8 and in this particular case, the 'Two-curve Intersection' method doesn't work in front view because the top entity is an arc

Thanks in advance to test it and confirm this fact


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

I wasn't being sarcastic, I was simply trying to point that we were talking about two totally different situations.

The original topic of this thread had already been addressed, 10 years ago, and the solution is still valid today. However, what you're talking about has never worked, period. In that case you need to provide some additional 'entities' since you're NOT offered any which are suitable for what you're attempting to do, pure and simple. I was never disputing that, only that ForrestAnderson's question had already been asked and fully answered.

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.

 

[PSI-CAD]

Hi John

Ok for the original Topic. But I have found that it's possible to find the intersection point and place the dimension in base view (no section view) with NX8.5 without creating a sketch . Is this true ?


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

Yes, you're correct. In NX 8.5 you can reference the 'Intersection Points' when creating a Cylindrical Dimension in a normal (non-section) Drawing view.

The reason for this is because in NX 8.5 when creating Drawing views, as part of a project to improve the performance of Drawing view updates and such, we are creating what could be considered as 'smart' extracted curves, but unlike in the past where an arc seen from on-edge would still be extracted as an arc, starting with NX 8.5 that on-edge view will now extract (in reality it's being projected) the arc as a line, and so now the Intersection Points can be found since the to curves selected will both be LINES.

Now that being said, what you first suggested in your post yesterday at 10:13 is in fact emulating what we now do automatically starting with NX 8.5 (you will note that with NX 8.5 the 'Extracted Edges' option on the Drawing view 'Style' dialog has been removed since it's no longer needed) so I have to admit, you had already stumbled onto something which was very close to what the software now does out-of-the-box. I'm sorry that I missed that nuisance until today as I had been focusing on a solution for the original situation, how to do this in the context of a Section View, an issue that we've already pretty well beaten to death ;-)

Anyway, your workaround is about the best for now with NX 8.0 (or NX 7.5 and NX 6.0 as well) when it's a non-section view, but even that will not be needed once you move to NX 8.5.

And one other thing, before you ask, in NX 8.5, even though that on-edge arc was extracted (projected) as a line, if for some other reason you still would like to reference the center of that 'circular' curve it will behave like an arc for those cases. So you're sort of getting the best of both worlds, something that behaves as a line when needed or as an arc when needed.

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.