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NX 6 Surface Finish? 1

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DesignJunkie

DesignJunkie

Aerospace
Feb 24, 2010
21
Hello,

I'm new to NX. Have used Inventor, Works and Pro/E in the past. I'm getting up to speed but I can't seem to figure out how to call out a surface finish in the drafting environment. I've checked the online help and searched this forum to no avail. I see that there are surface finish symbols available under Insert>Symbol>Custom Symbol, but I'm wondering if anybody knows an easier way...

Thanks!
 
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Hi again,

Just found the UG_env.dat file in the UGII folder. I turned the option for surface finish ON, only to discover that "Suface Finish Symbols are not supported in English partfiles or English Drawings." Since my company standard is in fact to use English units, I'm hoping somebody else has found a work-around?
 
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I've only ever used the Custom Symbol option.
Its not the most intuitive to use but you get used to it.

I guess ideally you would some kind of 'placeholder' that you could attach to the leg, and that you could assign a surface finish or gap or other symbol to.

TIP: If you come back to the drawing at a later date and want to change the surface finish symbol you don't have to delete the whole dimension. Just turn off the dimension legs (in the STYLE options) and turn them back on again. Same goes for gaps if you don't like where they appear.
 
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You can insert predefined 'Finish Symbols' as a Custom Symbol by going to...

Insert -> Symbols -> Custom Symbol...

...and in the Libraries section of the dialog select the 'Unigraphics Symbols' entry.

Or you could add the Finish Symbols directly to the model using the PMI module.

Note that in NX 7.5 we've added the Finish Symbols function directly to NX Drafting.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

To an Engineer, the glass is twice as big as it needs to be.
 
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Thanks guys,
Sounds like a note with a leader and the appropriate surface finish symbol grouped to the note is as good as it gets for NX6? I guess it'll have to do...
 
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I did not realize that the finish symbols were located in Insert -> Symbols -> Custom Symbol...
I have been using the user defined symbols.
When I go into "custom symbols" I do not see a way to add the finish symbol to a dimension extension line.
Is it possible to add a finish symbol to a dimension extension line the when using custom symbols?

 
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Unlike User Defined Symbols, Custom Symbols can not be included in a text string, at least not until NX 7.5.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

To an Engineer, the glass is twice as big as it needs to be.
 
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Jerry,

Can you explain how you use the user defined symbols to callout surface finish?
 
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Insert > symbol > user defined symbol > utility directory (on top) > scroll until you find finsh symbols (they all begin with "STS") > Use the four icons below to attach to a dimension, or place by themselves

The finish symbols that I use the most are STS_MAT_ and STS, but you will probably want to see what they all are by using the "standalone" icon and placing them on your drawing

If you attach the symbol to a leader, or extention line, be sure to use the symbols with the underscore at the end of their name.

You will be able to flip it using the mirror icons.

You can add these to a note. If you need help then just ask.

Using these may take a bit of trial and error, but you should be able to figure it out. Just ask if you need more help.
 
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I'm happy enough using custom symbols, but if you are going to use the older user defined symbols then seeding them into you drafting template files is a great way to go.

I just add them to the page and position them relative to a leader or face of the part more or less by eye. They're basically notes so I just make them positioned relative to the view. I guess what I'm saying is that keeping it simple suits me because I'm not using them so very frequently that taking the trouble to customise things appeals to me as an effective use of my time.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum
 
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Good point Hudson.

I look forward to when the finish symbols become more robust in 7.5
 
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One more thing. If you need to remove the finish symbol from an extention you will have to remove, then add back in, the extention line in the drafting menu ... rmc dimension > style

You also can add breaks/gaps to your extentions line in a similar manner:
 
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Jerry,
As the poster said in that link you gave above, "You da man!" Very helpful tips! I could have spent hours trying to figure that out. Thank you!
 
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If you and both a gap and finish symbol to an extention line then add the gap first, adjust the size, then add the finish symbol - because if you adjust the size of the gap while the finish symbol is on there too then the size of the finish symbol will change also.
 
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Har har,
Now I have something to contribute (even though it was my coworker that figured this one out). If you go to Edit>Component you can both move and/or delete a gap. Simply choose which action you'd like to perform then choose the dimension/object that has the gap in it. Works pretty slick.
 
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