Hello all,

I'm trying to emboss a usb icon onto a solid, without success.

The process I'm doing is this:

1. create the usb icon in Illustrator, export as DWG file.
2. import this DWG file in NX into the work part.
3. delete the cross hatching to be left with only the splines of the icon.
4. use the move tool to position and scale the icon where it should be.
5. use these splines to create an emboss feature on the main solid.

Upon creating the emboss feature, an error message says "new and changed faces or edges have failed geometry check. see syslog for details."

I've tried using the extrude tool instead, but the result is often warped/distorted surfaces on the extruded sides.

Surely this must be a common task, and in Solidworks I've not encountered problems with this. What is the correct procedure in NX?

NX8 i7-3770K@4.3Ghz 16GB Quadro2000

can you upload the USB .dwg file?

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

The procedure sounds OK, it is probably the input geometry that is to blame. Imported splines can cause problems, you can use tools such as info object (check degree, number of knot points, etc) or curvature combs (visualize curvature changes) to get more information on your spline. If you find problems your best bet would be to use the existing geometry as a guide and recreate it in NX.

www.nxjournaling.com

I would suspect open gaps in your geometry.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

I'm attaching the usb icon DWG file if anyone would like to replicate the problem.
I don't think there are gaps, because the extrude tool doesn't complain about gaps, although it creates warped surfaces as can be seen in the attached image.

Here is part of the output from the info>object :

Closure Status Open
Degree 3
Number of Poles 100
Number of Segments 33
Number of C0 Knots 32
Number of C1 Knots 0
Number of C2 Knots 0
Rational Status Polynomial
Defining Data None
Approximate rho -2418.61543561509

IMAGE:
http://files.engineering.com/getfile.aspx?folder=0...

DWG:
http://files.engineering.com/getfile.aspx?folder=0...

NX8 i7-3770K@4.3Ghz 16GB Quadro2000

Was able to import .dwg and set options for "Import Polylines As" to "Arcs/Lines" to get the results attached.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

• http://files.engineering.com/getfile.aspx?folder=fe34b972-8f1b-43d5-87a4-8f

What you are pointing to in the .png file looks like it should be the intersection of a line and arc, but I suspect it is really just a sharp kink in a spline.

www.nxjournaling.com

Have you checked the Reuse Library? There is a item titled 'Reuseable Object Library (Example Only)' and in it a folder named 'Mark' where you will find pre-created symbols for both LAN and USB as well as a general lettering feature. Also, there are many TrueType libraries which contain symbols of this type which can be used by the Geometric Text function which can then be used as construction curves for creating raised/engraved features.

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, I'm very curious how you achieved it. Did you create an emboss feature or an extruded subtract feature? And how did you import the DWG polylines as arcs/lines? I've tried that too, but when double clicking the resulting linework, I still get a spline (see attached image). Is this what you get too? And if you created an extruded subtract feature, how is the quality of the resulting surfaces? Are you for example able to create edge blends at the bottom of the extruded area?

NX8 i7-3770K@4.3Ghz 16GB Quadro2000

• http://files.engineering.com/getfile.aspx?folder=288c65c6-b1e1-4405-9661-3a

I was able to import it and use it both ways (splines | arcs\lines). When I double click I also get a spline (see attached). I used extrude and subtract. Can't edge blend most edges...there are a lot of small little curve oddities. I would re-create in sketch or use the re-use library as John suggest. One time I tried to use "Simplify Curve", it did create arcs and lines but still the same issue with blending.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

• http://files.engineering.com/getfile.aspx?folder=c27c2b8b-eb90-4798-b3e0-25

Here you go...works much better as a sketch.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

• http://files.engineering.com/getfile.aspx?folder=c3a879db-173e-4080-9b92-d3

Thank you John, creating a sketch from scratch in NX would be the ultimate solution. However, in many cases, you would have a more complex icon/mark/symbol/logo which you have created/modified in Adobe Illustrator, which then can be exported as DWG and imported into NX. But there is a problem with this workflow.

Here is a "workaround" to the problem.

It seems the NX DWG/DXF importer is unable to properly analyze a DWG file made in Illustrator (I don't know about DWG files made in Autocad yet), so that the DWG line entities are all converted into a single spline, which causes problems with extrude or emboss features. Now, in Solidworks this is not an issue because presumably Solidworks can analyze DWG files made with Illustrator because it converts the DWG straight line entities into "lines" and curved lines into "splines". Importing this Solidworks DWG into NX creates a group entity consisting of a correct mixture of lines and splines. Now extrude or emboss features can be created without problem.

So the workflow is now:

1. create customized icon/logo in illustrator. save as DWG.
2. import this DWG into a drawing in solidworks (select "convert to solidworks entities")
3. save this drawing as DWG again.
4. open this DWG in NX.

This solution involves using Solidworks as a go-between to correctly convert the DWG into a mixture of lines and splines. There are probably other programs that can do the same job.

Another solution for those who don't have solidworks, but it might fail in some cases:

1. create customized icon/logo in illustrator, then use the tool "cut path at selected anchor points" to cut all the anchor points in the drawing. save as DWG.
2. open this DWG in NX.
3. in case it fails, a solution might be to convert the imported entities with the "simplify curve" tool, however the problem is that it will split the original entities into a huge number of smaller lines and arcs.

NX8 i7-3770K@4.3Ghz 16GB Quadro2000

Note that there are also tools which will create TrueType and OpenType 'font' objects from Adobe illustrator objects, which can then be directly used inside of NX via the Geometry Text function.

http://www.ehow.com/how_5847999_convert-ai-ttf.htm...

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.

Thanks John, that is an even better method! I tried it with the demo version of Typetool 3 (cheapest software). The usb icon (which failed with the DWG import) now works perfect as a font glyph in the NX text tool. Both extrude and emboss can now be done without problem. A major advantage with this method is that as a font, the same symbols can be used in any graphics software as well, so it's a very neat way to organize/store all the icons.

You mentioned before that there are many truetype libraries with these types of icons. I've searched on google, but couldn't find any. I'm looking specifically for icons related to consumer products (power icon, battery icon, wireless icon, etc.)

NX8 i7-3770K@4.3Ghz 16GB Quadro2000

This is one site that I found which might have some of what you're looking for:

http://californiafonts.com/category/logos

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.