Rapid Dimension - NX9

[phillpd]

Creating a Rapid Dimension (Inferred) between a linear (in this case, vertical) edge and a Center Mark, why does it give me an Angular Dimension ?

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)

 

[JohnRBaker]

Can you provide some sort of example, perhaps a video or series of images?

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.

 

[carlharr]

If I remember right you have to pick the endpoint of the edge instead of the edge in the new rapid dimension.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[phillpd]

John,

I'm dimensioning from a vertical edge to the centreline of a hole. I was expecting a horizontal dimension, but only received a 0 degree angular dimension.

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)

 

[phillpd]

Image attached.

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)

 

[JohnRBaker]

This appears to be a problem and I'm going to open a PR to that effect. When I get some feedback, I'll post it here.

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.

 

[phillpd]

Thanks John.

If you switch from inferred to horizontal during creation, both objects are deselected and an alert appears.

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)

 

[Toost]

Here's another example of this odd behavior.
This one a "3D centerline" through a cylindrical face.


Regards,
Tomas

 

[carlharr]

Just checked, I did raise this back in December and I am fairly sure the solution is to select endpoint of the straight edge rather than the edge itself.

Unfortunately I can't check as I don't have 9 working at the mo.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[Toost]

That option isn't available in the example i provided due to the detail view. The workaround there is to switch to "horizontal".

Regards,
Tomas

 

[JohnRBaker]

So far the feedback that I've gotten indicates that it IS a problem (my PR was also not the first one) and that it's being worked on. If I get any additional info, I'll pass it along.

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.

 

[RyanVLee]

I opened a PR on this as well so it is known dropping the dialog of inhered to place one dimension then changing it back seems to fix it until you change out of drafting

Ryan Lee
Mechanical Project Engineer

NX 6.0.5.3
NX 9.0.1.3(Testing)
If you can think it it can be modeled

 

[JohnRBaker]

OK, I got some further clarification.

Technically the 'Inferred' dimension code is working correctly, well sort of. The problem is that if your first pick is either the 'Center Mark' symbol or the EDGE, the system thinks that you've selected two 'linear' references and if you've NOT told the system explicitly what it is that you're creating, i.e. you're in the 'Inferred' mode, it's logical to think that it's an angle, even IF the value is zero. For the vast majority of cases, when creating 'linear' dimensions, you are actually dimensioning between either two Points or a Point and an Edge (when we say 'Point' we mean a 'snap point' not necessarily an actual Point object). Now prior to NX 9.0 and the introduction of the so-called 'Rapid' dimension function, what happened was that we would let you select whatever you wanted and we would attempt to sort out whether you really needed to pick an edge or a point and while it work OK for most cases, there were a lot of instances where you had to resort to using an explicit dimension function to actually get what you wanted. That was because we couldn't always guess what it was that you SHOULD have selected, the Point or the Edge. A good example of this is when you wanted a Perpendicular dimension. It was virtually impossible prior to NX 9.0 using the 'Inferred' dimensions to create a 'Perpendicular' dimension, which is not a problem at all with the new 'Rapid' dimension even in it's 'Inferred' mode. The irony here is that while many people create 'Horizontal' and 'Vertical' dimensions, in reality they SHOULD have been creating 'Perpendicular' dimensions instead since that is what was really being dimensioned, the PERPENDICULAR distance between a Point and a linear Edge.

So the solution that is being worked on is that if your first selection is either a linear edge or 'Center Mark' symbol, we will force the second selection to be a snap point, unless you've explicitly said that you wanted an angular result. BTW, as mentioned already, that is the recommended approach that you should be using today. In other words, if you wish to dimension to a 'Center Mark' symbol and you've already selected a linear edge, place your cursor over the small 'crosshairs' portion of the symbol instead of one of it's radial lines (you'll know that you've got the correct 'point' because you will actually see the little 'feedback' icon showing that you've selected the 'Point' snap point of the symbol. That way the system will know that you're dimensioning it as if it were a 'Point' which is what you're doing anyway if you've already selected a linear edge as your first pick. Now if you pick the 'Center Mark' symbol first, then you need to pick the snap point, this will be the end-point in most cases, for your second pick. But if you really need a perpendicular dimension, which is going to be most of the time anyway, then pick the linear edge first and then the 'crosshairs' of the 'Center Mark' symbol for the second pick.

Anyway, I hope this explains better what's happening and how this will eventually be resolved, as well as being advised as to how to use the 'Rapid' function today to get what you consistently need to be getting when selecting 'Center Mark' symbols

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.

 

[phillpd]

Thanks for the explanation John.

The only issue with picking the 'point' of the Center Mark is that you won't get a gap between the Center Mark and the dimension line.

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)

 

[JohnRBaker]

I get the proper gaps on my system.

Make sure that you're getting the 'point' of the 'Center Mark' and not the center of the arc.

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.

 

[stephlouv]

Thanks a lot John.
But if the Rapid/Inferred (supposed to be intelligent) didn't give us satisfation or if it's too tricky to use.
We won't use it and we will ending with only 3 buttons in our dimension toolbar : Linear, Angular & Radial






"My english is bad ? That's why i'am french."

 

[JohnRBaker]

Like I said, most of the time Rapid Dimensioning is working exactly as intended, it's just this 'Center Mark' issue that was missed but it's being resolved. And as I also mentioned, now that we're actually taking into consideration what it is that you're selecting, edges versus snap points, NX can do a better job of creating the types of dimensions that it really should be creating, such as Perpendicular dimensions where in the past it tended to create more Horizontal or Vertical dimensions even when these were not always the best choice. Now NX can intelligently make those choices based on how and what you selected. This whole idea of calling it 'Rapid' was based on the assumption that people would leave it in it's default 'Inferred' mode and simply learn how to properly select the objects that are being dimensioned without having to constantly change the dimensioning 'Method'. Granted, there are still special situations where the 'Method' can't always be inferred, so we will continue to allow you to explicitly tell the Rapid Dimension function what 'Method' to use, as well as providing a full palette of specialize dimension types which cannot be reliably inferred no matter how 'smart' we make the software, such as Thickness or Arc Length or Chamfer, etc.

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.

 

[Toost]

So what you are saying, is that the fix will only be applied to "center marks" but not to 3D centerlines as in my example ?
- Since there is no point available on this one.
See attachment.

Regards,
Tomas

 

[JohnRBaker]

The current 'workaround' is to pick at least ONE point and since the 2D Centerline doesn't include a 'point', as you've pointed out, that means that you'll need to select a snap point on the 'frame' of you model. That being said, when they make the changes which are planned, they will account for 2D Centerlines as well as Center Marks.

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.

 

[phillpd]

Consider the attached image :

The 40 dimension is to the tangency of the arc. What I need.

The 39,21 is to the centre of the arc. Not what I need.

I can create the angular dimension only by selecting the 39,21 dimension ... selecting the 40 dimension throws an error.

NX 6.0.5.3
NX 9.0.2.5
Windows 7 64 (Windows 8.1 Tablet)