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scaling a sketch
- Thread starter UG39
- Start date
JohnRBaker
Mechanical
You can't scale a sketch, but you can scale whatever body, even if it's only a planar sheet body, that you create using the sketch.
If the sketch is simple, you could 'scale' each dimension of the sketch, but since you mention that this ia a 'logo' I suspect that this approach would not be practical.
What version of NX are you using?
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.
If the sketch is simple, you could 'scale' each dimension of the sketch, but since you mention that this ia a 'logo' I suspect that this approach would not be practical.
What version of NX are you using?
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.
If this is in modeling the Transform command might do what you need (it's an older command, depending on which version of NX you are using you might have to use the command finder to find it). If it's in drafting then create a symbol from it and then you can scale it each time you insert it into drafting.
Daniel Sikes
Design Engineer
Young Touchstone
NX 8.0.3.4
Daniel Sikes
Design Engineer
Young Touchstone
NX 8.0.3.4
JohnRBaker
Mechanical
Technically the old 'Transform' will work, up to a point. You can only scale the sketch curves and NOT the sketch itself which means that it's a copy, it's non-parametric and the resulting 'object' is no longer a sketch, but just bunch of individual non-grouped curves.
If you let us know what version of NX that you're running, we could provide at least some examples of what you might be able to do.
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.
If you let us know what version of NX that you're running, we could provide at least some examples of what you might be able to do.
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.
- Thread starter
- #5
Thanks for all reply
1st I am using NX10.
2nd working in modeling and logo in sketch format
with transform command can not be done in inactive mode
only in active mode possible if make scale with copy option (not move option), that is problem logo will doubled (and destination layer change does not work).
1st I am using NX10.
2nd working in modeling and logo in sketch format
with transform command can not be done in inactive mode
only in active mode possible if make scale with copy option (not move option), that is problem logo will doubled (and destination layer change does not work).
JohnRBaker
Mechanical
Can you provide at least a picture of what you're attempting to create as a sketch? Also, is the logo intended to be used in Modeling or on the face of a Drawing?
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.
- Thread starter
- #7
JohnRBaker
Mechanical
OK, what I did was go out on the web and found a free TrueType font that included the 'Plastic Recyle' symbols and the one I found was called 'FreeSerif' and it can be downloaded from a place called 'FONTS2U' located at:
I downloaded the font and once on my system, I was then able to use it to create a 'Text' curve feature of the '♳' symbol. Since this is a feature you have complete control over it's size by editing it. Now it is true that the 'PETE' part of the symbol will have to be added as a separate 'Text' curve feature but then their size could also be controlled parametrically so you willhave direct control over their size. To show you how this worked, I edited your part file (attached below) by duplicating your example symbol using TrueType fonts and the NX 'Text' curves feature function (note I grouped the two features into a Feature Group just to make it easier to manage them. So for reference, the symbol was created using the FreeSerif font and the 'PETE' text using Arial with a 'Bold' option.
Anyway, take a look and let me know what you thin.
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.
I downloaded the font and once on my system, I was then able to use it to create a 'Text' curve feature of the '♳' symbol. Since this is a feature you have complete control over it's size by editing it. Now it is true that the 'PETE' part of the symbol will have to be added as a separate 'Text' curve feature but then their size could also be controlled parametrically so you willhave direct control over their size. To show you how this worked, I edited your part file (attached below) by duplicating your example symbol using TrueType fonts and the NX 'Text' curves feature function (note I grouped the two features into a Feature Group just to make it easier to manage them. So for reference, the symbol was created using the FreeSerif font and the 'PETE' text using Arial with a 'Bold' option.
Anyway, take a look and let me know what you thin.
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.
- Thread starter
- #9
Using a sketch isn't necessary. We have a small library of such symbols saved off as dumb curves; when needed, we add them to our current model, scale them as necessary with the transform command and extrude them to engrave/emboss the part as needed.
If you really want to stick with sketches, you can build the scale factor into the sketch definition. Create an expression such as "recycle_scale = 1" (type: constant) and multiply each of your sketch dimensions by this scale factor. The user of the sketch logo would have to know about and change the "recycle_scale" expression for proper use...
www.nxjournaling.com
If you really want to stick with sketches, you can build the scale factor into the sketch definition. Create an expression such as "recycle_scale = 1" (type: constant) and multiply each of your sketch dimensions by this scale factor. The user of the sketch logo would have to know about and change the "recycle_scale" expression for proper use...
www.nxjournaling.com
PrintScaffold
Mechanical
A sidenote - although in the feature tree we observe multiple Scale body features, they are created automatically from a single tool calling event. So the process is quite robust.
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