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Adding custom reuse library part to ass'y with "clone option", NX9 2

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3dr

3dr

Automotive
Jul 10, 2004
456
Is there a way to do this and be able to name the part yourself at insertion? Perhaps even have a "prefix" added to the actual file name automatically?? That's even better.

I've been prowling the internet and help files for a pathway to something like this, with no luck.

Using "Make Unique" after insertion is getting old and I don't want to use part families, it's to restrictive.
My parts have to many options to make that practical.

What I need is to be able to preserve my library parts in one place so multiple people can use them.
We can't do that right now. With the method I'm using, if you forget to "Make Unique" before modifying it, the original part in the library part is then messed up.

TIA

Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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Have you considered turning your reuse parts into model templates?

You'd have to create a .pax file for all the parts of interest, but when you perform a 'save', NX will prompt for a file name for the new parts derived from the template (the template files will NOT be overwritten). I think you can even specify a default prefix and/or suffix for the file name.

Alternately, perhaps just changing the file permissions to read-only on your current reuse parts would do the trick.

www.nxjournaling.com
 
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Yeah, I looked at that just this morning. It works fine but you can't mate or place the part that way.

It just places the part at 0,0,0. Also, it doesn't allow for renaming the part within a small assembly. Only the top level part.

I may have try it until I find the something better tho.


Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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3dr said:
It works fine but you can't mate or place the part that way. It just places the part at 0,0,0.
Click to expand...

I'm pretty sure this behavior can be changed. Check the customer defaults: Assemblies -> General -> component operations -> {single/multi select drag and drop options}.

www.nxjournaling.com
 
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It doesn't look like any of those fields apply to to "make new" part.

Am I missing something??

Being able to turn that functionality on could be a big leap forward!

Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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I'm not sure that I understand this correctly.

- You have a number of standard articles that you want to be able to drag drop into assemblies, and these details should be cloned/ modified to suit / and the master should not be used as is.
Correct ?

If so, that is what the "reusable components" do with the exception that one has to toggle "Clone" on each addition. ( it defaults to "Reference" which is the same as "add the master without the save as".

To set this up, Customer defaults - Gateway -reuse lib - General ( i assume you run without Teamcenter) -
add in the "native NX" field something similar to: Fasteners|D:\my_parts where "fasteners" is the directory which will show up in the reuse tab in NX , the separator "|" between the name and the directory.
repeat on new line for the next standard directory.

Then make your standard parts readonly.

Regards,
Tomas

 
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Ok...

Toost said:
- You have a number of standard articles that you want to be able to drag drop into assemblies, and these details should be cloned/ modified to suit / and the master should not be used as is.
Correct ? Yes Exactly

I sense I'm getting close. I've done as directed but I'm still falling short.

1. Created and set directory in --> Cust Defaults: Gate, Reuse Library, General, Native NX (Field)
Smart|C:\NX_Lib\Smart Parts
2. Copied a dozen sample parts into the above folder and set their file properties to "read only"
3. Restarted NX, Opend an ass'y, dragged one the sample parts out of the "Smart" Reuse library and placed it.

But I just get the standard "Add Component" Dialogue

What am I missing? Should I have a KRX even tho I'm not doing a part family? Am I missing a setting in customer defaults?


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3dr (Automotive) (OP)
7 Jan 15 18:05
Is there a way to do this and be able to name the part yourself at insertion? Perhaps even have a "prefix" added to the actual file name automatically?? That's even better.

I've been prowling the internet and help files for a pathway to something like this, with no luck.

Using "Make Unique" after insertion is getting old and I don't want to use part families, it's to restrictive.
My parts have to many options to make that practical.

What I need is to be able to preserve my library parts in one place so multiple people can use them.
We can't do that right now. With the method I'm using, if you forget to "Make Unique" before modifying it, the original part in the library part is then messed up.

TIA
Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1


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this post

cowski (Mechanical)
7 Jan 15 19:12
Have you considered turning your reuse parts into model templates?

You'd have to create a .pax file for all the parts of interest, but when you perform a 'save', NX will prompt for a file name for the new parts derived from the template (the template files will NOT be overwritten). I think you can even specify a default prefix and/or suffix for the file name.

Alternately, perhaps just changing the file permissions to read-only on your current reuse parts would do the trick.

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3dr (Automotive) (OP)
7 Jan 15 20:03
Yeah, I looked at that just this morning. It works fine but you can't mate or place the part that way.

It just places the part at 0,0,0. Also, it doesn't allow for renaming the part within a small assembly. Only the top level part.

I may have try it until I find the something better tho.
Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1


Red Flag
this post

cowski (Mechanical)
7 Jan 15 20:28
Quote (3dr)
It works fine but you can't mate or place the part that way. It just places the part at 0,0,0.

I'm pretty sure this behavior can be changed. Check the customer defaults: Assemblies -> General -> component operations -> {single/multi select drag and drop options}.

Like this post?
Star it!


Red Flag
this post

3dr (Automotive) (OP)
8 Jan 15 14:20
It doesn't look like any of those fields apply to to "make new" part.

Am I missing something??

Being able to turn that functionality on could be a big leap forward!
Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1


Red Flag
this post

Helpful Member! Toost (Mechanical)
8 Jan 15 16:49
I'm not sure that I understand this correctly.

- You have a number of standard articles that you want to be able to drag drop into assemblies, and these details should be cloned/ modified to suit / and the master should not be used as is.
Correct ?

Toost said:
If so, that is what the "reusable components" do with the exception that one has to toggle "Clone" on each addition. ( it defaults to "Reference" which is the same as "add the master without the save as"
Click to expand...
I can't make heads or tails our of this comment, I'm just not seeing what I have to do to achieve this

TIA

Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
Click to expand...
 
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Ok Toost, Sorry for the crazy post... tried using the "quotes" tool and butchered it.

"You have a number of standard articles that you want to be able to drag drop into assemblies, and these details should be cloned/ modified to suit / and the master should not be used as is.
Correct ?" Yes Exactly

I sense I'm getting close. I've done as directed but I'm still falling short.

1. Created and set directory in --> Cust Defaults: Gate, Reuse Library, General, Native NX (Field)
Smart|C:\NX_Lib\Smart Parts
2. Copied a dozen sample parts into the above folder and set their file properties to "read only"
3. Restarted NX, Opend an ass'y, dragged one the sample parts out of the "Smart" Reuse library and placed it.

But I just get the standard "Add Component" Dialogue and I'm not seeing where I can toggle to "Clone"

What am I missing? Should I have a KRX even tho I'm not doing a part family? Am I missing a setting in customer defaults?

"If so, that is what the "reusable components" do with the exception that one has to toggle "Clone" on each addition. ( it defaults to "Reference" which is the same as "add the master without the save as"
I can't make heads or tails our of this comment, I'm just not seeing what I have to do to achieve this

TIA
Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1

Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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So, after some diligence, I've realized I need to create a reusable part or I won't get the cloning capability. After looking it up it appears that I can make a reusable part without it being a "part family" part. Is this correct?

Also, while making changes in customer defaults I must have accidentally deleted something. I cant drag anything into the ass'y from the reuse libraries without getting this message
Reuse Library Error
"The family member saving directory does not exist"

It's been so long since I've set this up I'm having trouble finding it.
I think I may have deleted a line in
Gateway, Reuse Library, General
Reuse Library Configuration File
"Windows "Field"

I'm pretty sure I had something in there before. Any help?

TIA



Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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Dave --

I heard about a similar error recently (earlier this week, in fact), and got a response to this effect from the Reuse Library developers:

In a previous release, the Part Family Save Directory was set to $Windows/Program Files/ReuseLibraryFamilyMember by default. On the WinX64 platform, there appear to be times when NX cannot create this folder under the "$Windows/Program Files" folder branch -- we suspect because of a security-driven limitation on write access. Changing this customer default setting to a writable location can eliminate the error:

150108_reuse_library.jpg


Does that fix the problem for you?

Taylor Anderson
NX Product Manager, Knowledge Reuse and NX Design
Product Engineering Software
Siemens Product Lifecycle Management Software Inc.
(Phoenix, Arizona)
 
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Oops, sorry . I forgot to mention the magical stuff.
When you have a part i this directory, open the reuse tab , select the new part in the "Member select" field, RMB create KRX.
You can in this dialog specify a preview image, select a spreadsheet ( which might contain default values) and also specify a member save directory, and setup the dialog that will be used when using the model. There is also an option for auto matching,- if you drop a screw onto a hole, = "select next smaller size".

But, if all you do is create the krx without any options, you get the clone option. -i.e, create krx+ok.

Attached is an example i helped another fellow with on this forum sometime ago. Unzip in your reuse library.
The spreadsheet is really simple, i think it's self explanatory.

Also note that you can, as in the example, setup a number of default values, but that you always can override these by double clicking in the "details" field, example the attached Grate is default 1000/1200/1225/1500 but double click the "Grate_length" and you can enter any number.

Regards,
Tomas
 
 http://files.engineering.com/getfile.aspx?folder=1b4eacb0-74f6-47a5-b4fa-25729a729c66&file=Grate.zip
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Thanks!
I solved all the issues I posted for late last night. Now that I see how this can be done... I'm jacked about converting all my stuff over.

Wish I would have done a little more research before I made my parts library tho. Now I have to untangle tons of expressions from the attribute system that I was effectively using as my GUI.
But the power gains are well worth it.

I know I'm going to need to understand the spread sheet formatting for this better... some of my parts are tricky with a lot of options. Some to make the part, some for the subtraction bodies.

These are few things I need to understand before moving fwd.
1. I would like to create a break in the drop down options that define the part.. between the part variables & subtraction body variables. (So things don't "run together")
2. How do I present a variable name "Label" that's different than the expression name. I will need some flexibility here I think.
3. When have 3-4 part ass'y to drag in, will it clone the whole thing? And I assume all the Variables that control it need to be at the top level part?? (This one I'll be waiting to tackle!)

Are there any resources for this?

TIA





Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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I can't answer all you questions. If Taylor Anderson is still listening i think he can reply on 1).
2) Create an .xls ( or xlsx) this should look like this:
PARAMETERS
"Part Name" "expression1" "expression2"

END

In the KRX edit dialog, move the expressions you like to present from left to the right window, then double click the
 
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Toost said:
move the expressions you like to present from left to the right window, then double click the...
Click to expand...

And tune in next week for the thrilling conclusion!
 
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Well, if i click Submit Post instead of Preview, only half the message gets posted...

The spreadsheet dictates what expression can be presented in the NX dialog.
so the variables that you add can be edited through the NX dialog. - you can omit things like extrude start distance if this is always 0 by not including that expression in the spreadsheet.
If your variables has "poor" names, such as "p0" there is a possibility to change this,
see attached image.
Continued from above :
In the Krx dialog, move the expression you like to rename( erratic in above post) from the left to the right, then double click the descriptive name. ( see image.)
Note that all expressions in the spreadsheet will be listed in the details field but only "expressions in the right field" will be presented in the "Primary parameters".
( The reason all variables in the picture have a "blank value" in the image is that the spreadsheet doesn't have any values.)

You can , for casting type reuse parts have a both positive and negative add, for example adding a slider in a mold tool should both add the slider and cut a fitting pocket. model the pocket in the standard part, add the "pocket" to a reference set named "false". ( the ref set name can be set in customer defaults) - Thereby the option "Pocket".

Regards,
Tomas
 
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Thanks Toost!
I'm well on my way to converting my library. I actually had to work on Friday but I did some weekend time on this task and it's working out better than I even hoped. The pocketing tool is great!
Assemblies do fully clone so even that concern is gone.

Now, howabout this one...
I've got a spring that has 3 inputs.
1. Diameter
2. Wire Diameter
3. Length

The list of available lengths needs to change up depending on selection the combo of #1 & 2

Is there a way to nest the spread sheet selections to accommodate this?
It seems to me that the re-use screws do this so I'm thinking it can be done. I've been looking for those spread sheets and can't find them.

TIA



Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1
 
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The reusable screws from the "Machinery library" are all "Part families", - The spreadsheet is inside the template part.
I assume that one can do the same with the reuse spreadsheet, i think its a matter of adding as many lines in the spreadsheet as there are variants.

regards,
Tomas
 
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