making new KE nx reuse library parts

stephangeurts · Dec 4, 2012

dear people,

i have a problem with making new parts for the reuse library NX7.5.
i make the part, say a box 40x40x40.
with tools>expression i link the value with a excel sheet.
i save the part and axcel file in the same location.
with NX i create a .krx file.
i can load the .krx file in a new file as its suposed to, but when i put the same part with other value's in, they both chance.
my question is: how can i use the same part with different value's?.
is it a setting i have to chance?

i hope to hear from you,

a fellow engineer.

ps: i'm sorry if there was allready the same post, i have searched for it but haven't found the solution.

Toost · Dec 4, 2012

The same part cannot have two or more "values" in the same session. - It is one part.
The reuse library "expects" you to have the KRX etc create a new part per "size".
I.e, If you desire to have an M4 screw in the same session as a M8, You need two screw parts.

Regards,
Tomas

stephangeurts · Dec 6, 2012

hi Tomas,

i understand that its not possible to have the same part with 2 diffente value's, but i wonder if its possible to let NX automaticly create a new part when u load another one in. so you can hav multiple values.

Regards,
Stephan

cubalibre000 · Dec 6, 2012

The solution is Deformable Part.
Starting to NX8.5, Reuse Library support them.

Thank you...

Using NX 8 and TC9.1

Toost · Dec 7, 2012

Stephan, can you describe what it is that you want to accomplish ?
It is fully possible to have NX clone parts when adding them via the reuse library. ( Clone = make copy of)
Or, if you add components, your spreadsheet can be prepared with "new filenames" such as that when you select say "40 mm", then NX will open or create the new part. ( Open if it exists already.)

Regards,
Tomas

swale74 · Dec 7, 2012

Here is a good example. I would like to add this part to the reuse library and then when required I would like to pull this and adjust the length and width to create the grate required in the assembly. The issue is sometimes multiple size are required in the assembly and i also can't figure out how to insert multiple custom sizes. I'm running NX 6.0.5.3
Manually cloning this part each time you need it is the best solution I've found. Tomas you say there is a way to get NX to clone from the reuse library? Or do you mean add the first part and then clone copies from the assembly parts for the different sizes?

Help please!

NX 6.0.5.3 in Windows 7
Mechanical designer

Toost · Dec 7, 2012

I don't remember all the details at the moment on how to set these up, it's friday and i have 200 km's to drive home....
The attached picture is a screenshot from NX6 and the Machinery library ( The free Siemens download)
When using the specific profile, one can tick the clone option and be prompted to enter/accept a filename.
I had a look in the corresponding spreadsheet, and there is no "predetermined filename" column, only the "sizes" of the I-beam.

Maybe somebody remembers the details, or i can look it up later...

Regards,
Tomas

Toost · Dec 7, 2012

-Dang! Once triggered i just can't keep my fingers off....
Here's how:
1) create a new directory ( of which which you remember the exact name, -keep the window open.)
2) in NX :File - utilities - Customer defaults- gateway - reuse library - enter "Grates|"the directoryname from above"" Save the customer defaults by OK.
3) Exit NX, and restart NX.
4) unzip the attached zipfile in the new directory.
5) open or create a new part in NX. Open reuse tab, select the grate directory and in the lower part select the grate, drag drop into graphics.
( If the above is done in a slightly erratic order, the grate part will not be visible until one does a "refresh" in the reuse library, or starts a new session.)

If you want, you can edit the spreadsheet as desired, i have only included two of the variables from the part since i guessed that these two were of interest.
Right click the "grate preview" in the lower area and select edit KRX to change the details.

Regards,
Tomas

stephangeurts · Dec 9, 2012

hey Tomas,

this is exactly what i asked for, thanks alot. i noticed that when u clone, the clone will be saved at a directory, lets say C://windows/. and i want it to be to, lets say U://reuse_library.
i have looked ad utilities>gateway>reuselibrary and i cant find the clone options and directory for the clone. do you know a way to chance that, or somebody else.

thanks alot allready,

regards,
Stephan

stephangeurts · Dec 9, 2012

find it allready!!!.

everybody thanks alot.

with kind regards,

Stephan Geurts

stephangeurts · Dec 10, 2012

one last question

,

i want that NX gives my clone part automaticly a name, so lets say my part name is I beam, i choose the values 40X5X5. i want my part to name I_beam40x5x5_001 and when i clone the same part it has to turn out to I_beam40x5x5_002. i hope u guys understand.
i have tried to do it with Excel but it didnt worked out. is there another way? or is it a dead end?

i hope to hear from u soon,

with kind regards,

Stephan Geurts

Toost · Dec 10, 2012

I normally run under TC, so i get a little puzzled on this issue. See attached image.
When running with TC it is possible by adding an extra column where one can set a "proposed name". ( I hope you noted that you can change / override the values from the spreadsheet by double click on the line with the padlock symbol ?)

Regards,
Tomas

stephangeurts · Dec 11, 2012

Hey Tomas,

i run Teamcenter to, sorry for not telling it. i noticed that when u choose clone you can asses to a window that allows u to chance the partname and directory (not sure u mean this with your last respons). the only thing about this is i want it to be automatticly. there is a box named Name rule with "<template_name>_???" in it. i think it has to be done with this but i dont know how. i tried somethings. i hope you follow me. I hope i made myself clear.
it would be wonderful if this all workes out.
thanks alot allready,

regards,

Stephan

swale74 · Dec 11, 2012

Stephan, I think what you're looking for can be found here(see image). Under the Reference/Clone see Part name management. Add the variable digits to the naming. eg <Beam_Width>_<Beam_Thick1>

Thanks Tomas this is exactly what I needed and now hopefully I can build on this.

NX 6.0.5.3 in Windows 7
Mechanical designer

crecore · Dec 11, 2012

Maybe I am missing something but why not just create a part family master file (driven by a spreadsheet), then create all of the parts, then create the krx files from those parts?

NX 8.0.1.5

stephangeurts · Dec 11, 2012

hey swale74,

i dont quite follow you. i can find the part name management, but i cant let the part name rule work.
even when this work. will this be working with only this part or with all Re-use parts.

my part is named "gelijkzijdige T profiel warmgewalst" sorry its dutch
i have 4 parameters: A B D and r.
so i have made this: <gelijkzijdige T profiel warmgewalst_000>_<A>_<B>_<D>_<r>
when i make a clone part i get this: gelijkzijdige T profiel warmgewalst_000_A_B_D_r
while i want this: gelijkzijdige T profiel warmgewalst_000_20_30_5_3
i hope i made myself clear,

regards,

Stephan

Toost · Dec 12, 2012

Crecore,: If we would use Part Families, we would have to predict all possible variants and options in advance and define these in the spreadsheet.
The point in using this method is that we can on the fly define new variants which aren't predefined in the spreadsheet, and in the end save as a new part.
Using part families, the Expression values defined in the spreadsheet must be edited from that master spreadsheet, this method allows us to change the values on the fly.

Stephan,: I doubt that the naming method will work. The "<template_name>_???" is defined in the customer defaults under Gateway- Reuse library- ..naming.. and applies to all reusable parts ( that is cloned), it simply means "<get name of template> then underscore "_" and add 3 digits to the end, starting with 001"

A possible workaround could probably be that you define an expression in the reusable template that "collects" up the values from A,B,D,r and presents the result as a string in the menu, which you could copy-paste as the new part name, see attached image.

Regards,
Tomas

stephangeurts · Dec 12, 2012

hey Tomas,

yeah that workes out to but wouldnt it be nice if it could be automaticly

. if i find another way i will let you know. for now i will do it with this, im allready glad that i can clone parts

thanks everybody,

with kind regards,

Stephan Geurts

PDW · Dec 12, 2012

Hi Stephan,

a question, nothing to do with this toppic...
Are you Dutch/Flemish working in Flanders or Holland?

Kind regards,
Pascal

Best regards,

Pascal,

NX8 and waiting for NX 8.5, on Win7 64 Bit

stephangeurts · Dec 13, 2012

hey Pascal

im dutch working in holland.
why you ask?

regards,

Stephan Geurts

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