NX7.5 Drag dimension in sketch to modify its value
NX7.5 Drag dimension in sketch to modify its value
(OP)
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.





RE: NX7.5 Drag dimension in sketch to modify its value
Hold "Shift" key, select with MB1 the geometry that you want to modify and drag it!
MZ7DYJ
RE: NX7.5 Drag dimension in sketch to modify its value
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.
RE: NX7.5 Drag dimension in sketch to modify its value
Thank you
PD: John, do you have a twitter account or other channel providing info or news about NX?
RE: NX7.5 Drag dimension in sketch to modify its value
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
RE: NX7.5 Drag dimension in sketch to modify its value
You could try:
http://blog.industrysoftware.automation.siemens.co...
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: NX7.5 Drag dimension in sketch to modify its value
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.
RE: NX7.5 Drag dimension in sketch to modify its value
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.
RE: NX7.5 Drag dimension in sketch to modify its value
John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1
RE: NX7.5 Drag dimension in sketch to modify its value
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: NX7.5 Drag dimension in sketch to modify its value
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.