Rapid Dimension - NX9
Rapid Dimension - NX9
(OP)
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)





RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
www.jcb.com
NX 7.5 with TC 8.3
RE: Rapid Dimension - NX9
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)
RE: Rapid Dimension - NX9
NX 6.0.5.3
NX 9.0.1.3
Windows 7 64 (Windows 8.1 Tablet)
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
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)
RE: Rapid Dimension - NX9
This one a "3D centerline" through a cylindrical face.
Regards,
Tomas
RE: Rapid Dimension - NX9
Unfortunately I can't check as I don't have 9 working at the mo.
www.jcb.com
NX 7.5 with TC 8.3
RE: Rapid Dimension - NX9
Regards,
Tomas
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
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
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
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)
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
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."
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
- Since there is no point available on this one.
See attachment.
Regards,
Tomas
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
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)
RE: Rapid Dimension - NX9
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.
RE: Rapid Dimension - NX9
I hope that's going to be fixed in a 9.0.2 MP ... we're reliant on that for our product portfolio.
NX 6.0.5.3
NX 9.0.2.5
Windows 7 64 (Windows 8.1 Tablet)