JuanNavarroSanz
Mechanical
- Oct 25, 2012
- 11
Is it possible to pick and drag dimension in sketch to modify its value. I'm only able to draw the dimension text.
Thank you.
Thank you.
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NX7.5 Drag dimension in sketch to modify its value 1
- Thread starter JuanNavarroSanz
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JohnRBaker
Mechanical
If you're talking about 'dynamically' editing the numerical value of an EXISTING Sketch dimension, try going to...
Edit -> Sketch Parameters...
...and when the dialog opens, select the Dimension-of-interest and you then be able to use the 'slider' at the bottom of the dialog to dynamically alter the value of the Sketch dimension.
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.
Edit -> Sketch Parameters...
...and when the dialog opens, select the Dimension-of-interest and you then be able to use the 'slider' at the bottom of the dialog to dynamically alter the value of the Sketch dimension.
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.
-
1
- Thread starter
- #4
JuanNavarroSanz
Mechanical
- Oct 25, 2012
- 11
I'm transitioning from IDEAS, where there is a way to dynamically drag a dimension (via the drag tool) thus driving the sketch, I understand there is no way to do this in NX different from Edit -> Sketch Parameters...
Thank you
PD: John, do you have a twitter account or other channel providing info or news about NX?
Thank you
PD: John, do you have a twitter account or other channel providing info or news about NX?
cubalibre000
Mechanical
Starting from NX7.5, auto-dimension in sketch, dimension automatically all entities in the sketch to become fully virtually constrained.
Virtually because you can drag&drop entities, not dimension as in Ideas.
If you add dimension, NX remove auto-dimension that over constraints the sketch.
If you enter the auto-dimension because NX has dimensioned well you sketch, the dimension become real.
Thank you...
Using NX 8 and TC9.1
Virtually because you can drag&drop entities, not dimension as in Ideas.
If you add dimension, NX remove auto-dimension that over constraints the sketch.
If you enter the auto-dimension because NX has dimensioned well you sketch, the dimension become real.
Thank you...
Using NX 8 and TC9.1
JohnRBaker
Mechanical
JuanNavarroSanz said:
You could try:
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.
- Thread starter
- #7
JuanNavarroSanz
Mechanical
- Oct 25, 2012
- 11
Finally I found a solution to drag and redimension a dimensionally constrained sketch, very useful to redimension a part that is in a preliminar stage (shape defined, but not exact dimensions).
I adopted this while learning Catia. In Catia it is posible to freely drag a line in a sketch that is fully constrained, by pressing shift and dragging the geometry. While the shift key is pressed the dimensions are TEMPORARY set as reference, thus not locking the geometry... so the solution in NX is to convert the dimension (unfortunately manually) to reference, drag the geometry, see the result, or adjust the part aproximately, and then finally convert the dimension to driving an provide a exact value.
An temporary-reference feature like catia's one will be nice.
I adopted this while learning Catia. In Catia it is posible to freely drag a line in a sketch that is fully constrained, by pressing shift and dragging the geometry. While the shift key is pressed the dimensions are TEMPORARY set as reference, thus not locking the geometry... so the solution in NX is to convert the dimension (unfortunately manually) to reference, drag the geometry, see the result, or adjust the part aproximately, and then finally convert the dimension to driving an provide a exact value.
An temporary-reference feature like catia's one will be nice.
JohnRBaker
Mechanical
Or you could just work with Auto Dimensions toggled ON, drag your geometry until the numbers are what they need to be to meet your design criteria and then convert the Auto Dimensions into Driving Dimensions by simply double-clicking the Auto Dimension and hitting 'Return'.
If later you wish to 'drag' rather then edit a numerical value, simply delete the Driving Dimension, which will then be replaced once more by an Auto Dimension and repeat the above described workflow.
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.
If later you wish to 'drag' rather then edit a numerical value, simply delete the Driving Dimension, which will then be replaced once more by an Auto Dimension and repeat the above described workflow.
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.
wackolacko
Automotive
This option will work (see pic) if you create your dimensions manually.
John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1
John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1
JohnRBaker
Mechanical
I already described that approach back on 29 November ;-)
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.
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.
- Thread starter
- #11
JuanNavarroSanz
Mechanical
- Oct 25, 2012
- 11
Thank you again John.
Im reluctant to someone (call it NX) over my shoulder putting dimensions in my sketch as im drawing it, but, your solution is good in a way, i can freehand draw my sketch, fully dimension it, then turn on continous auto dimensioning, then erase the dimension to drag, it becomes an auto dimension (dark red), drag, double click it, and hit return... but definitively is a difficult way to achieve something solved in catia with a keystroke or in ideas (from where im transitioning) with the drag feature.
Im reluctant to someone (call it NX) over my shoulder putting dimensions in my sketch as im drawing it, but, your solution is good in a way, i can freehand draw my sketch, fully dimension it, then turn on continous auto dimensioning, then erase the dimension to drag, it becomes an auto dimension (dark red), drag, double click it, and hit return... but definitively is a difficult way to achieve something solved in catia with a keystroke or in ideas (from where im transitioning) with the drag feature.
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