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NX9 - Sketch Dual Dimensions
- Thread starter phillpd
- Start date
JohnRBaker
Mechanical
Not as a 'driver' dimension, which is what Sketch dimensions are. Now you might be able to create non-dirveing or 'driven' dimensions (known as 'Reference' dimensions in the Sketcher) which would allow this, but a 'driver' dimension can only be used with one unit scheme.
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.
JohnRBaker
Mechanical
While in the Sketch, select the Dimensions, press MB3, select Settings and you'll find a 'Dual' option.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
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.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
JohnRBaker
Mechanical
I've looked further into this issue and there actually is a way to get what you want.
Lets say you're creating a Sketch in a Metric part and you added dimensions to the sketch, which defaults to being shown as Expressions. If you then change the display of the dimensions to show dual dimensions you'll see the same EXPRESSIONS in both the upper and lower dimensions even if you had set the secondary units to Inches. Now finish the sketch and select it on the screen, press MB3, selecting the 'Settings...' option and change the 'Dimension Label' to 'Value' instead of 'Expression'. Now go back into your sketch and you'll see that you now have true 'Dual Dimensions' inside your sketch. Note however that you're NOT seeing the expressions but rather the values of the dimensions and when you go to edit a sketch dimension it will use to the actual expression value, which will be in the models base units.
BTW, even if you don't do what I did above, but leave your sketch dimensions with metric over metric format, if you indicate that you want to show the Dimensions as PMI, when you leave the sketch you'll see true 'Dual Dimensions'.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
Lets say you're creating a Sketch in a Metric part and you added dimensions to the sketch, which defaults to being shown as Expressions. If you then change the display of the dimensions to show dual dimensions you'll see the same EXPRESSIONS in both the upper and lower dimensions even if you had set the secondary units to Inches. Now finish the sketch and select it on the screen, press MB3, selecting the 'Settings...' option and change the 'Dimension Label' to 'Value' instead of 'Expression'. Now go back into your sketch and you'll see that you now have true 'Dual Dimensions' inside your sketch. Note however that you're NOT seeing the expressions but rather the values of the dimensions and when you go to edit a sketch dimension it will use to the actual expression value, which will be in the models base units.
BTW, even if you don't do what I did above, but leave your sketch dimensions with metric over metric format, if you indicate that you want to show the Dimensions as PMI, when you leave the sketch you'll see true 'Dual Dimensions'.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
Hi John,
When I MB3 on the dimensions, I am not getting the "DUAL" option as you mentioned. (see attached image). Is there a place to permanently turn off dual dimensions for Sketcher? I think most companies work in a single unit - seems like the default for Sketcher could be set to just the unit you're designing in?
When I MB3 on the dimensions, I am not getting the "DUAL" option as you mentioned. (see attached image). Is there a place to permanently turn off dual dimensions for Sketcher? I think most companies work in a single unit - seems like the default for Sketcher could be set to just the unit you're designing in?
Ooops, sorry.
MB3 DOES take me to settings, where you can toggle off "Dual" for dimensions that you select.
But I don't want to have to do this every time I start a Sketch...
Hoping for a Customer Default or setting somewhere to never invoke "Dual Dimensions" in Sketcher.
MB3 DOES take me to settings, where you can toggle off "Dual" for dimensions that you select.
But I don't want to have to do this every time I start a Sketch...
Hoping for a Customer Default or setting somewhere to never invoke "Dual Dimensions" in Sketcher.
Sketch dimensions use your dimension preferences. For existing parts, change your annotation preferences. For new parts change your customer defaults and/or your template files.
www.nxjournaling.com
www.nxjournaling.com
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