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The NX Machinery Library 

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In this NX A to Z article I will discuss the NX Machinery Library, which is essentially a standard parts library that can be downloaded from Siemens by any active NX customer. I will explain how to download and install it, how to share it with all of the NX users in your company and how to add the standard parts to your NX assemblies.

Downloading and Installing the Library

The first step obviously is to download the library from Siemens support website. So, click the link below and then click on Download files as shown in the image.

Siemens GTAC

You will be required to login using your webkey account credentials. If you don’t have a webkey account, take a look at the NX A to Z article on Installing NX to learn how to set one up. Once you have logged in, you will be directed to the Siemens PLM FTP Server. From there, click on the link for All Siemens PLM Products. On the next page, click on the NX/Unigraphics NX tab, select your operating system and then scoll down to the Machinery Library section as shown below.

There are essentially two components to the Machinery Library – the library install tool and the libraries themselves. The first step is to download the library install tool, which is shown below.

Once you have that downloaded, then you can download as many libraries as you want. It is best to select the newest version of each library and you need to be using NX 5 or later to use the machinery library. You can download the install tool and the libraries to any location on your computer or your network. You should also download Machinery-Library-readme.doc (explains how to start the install tool).

One you have the install tool and the libraries that you want downloaded, unzip the install tool – don’t unzip the libraries – and then open the NX_Machiery Library Install - User Guide folder and in this folder are the install instructions. Which basically consist of the putting the zipped up libraries in the NX_Machinery Library Install - kits\tool\libs folder and then running MachineryLibrary-Installation.bat.

The only thing to be aware of is that if you want everyone at your company that is using NX to access the same instance of the library (makes updates easier and makes any customizations available to everyone) then you need to install the library on your network, not on your local hard drive.

Once you have installed the library, you should have a folder like this wherever you elected to install it.

I have the ANSI Inch, ANSI Metric and ISO libraries installed. You can always add more libraries and/or update the libraries you have anytime and you don’t need to keep the install tool on your computer – you can put it on a USB or just download it again when you need to do an update.

Connecting the Library to NX

Now that you have installed the library, you need to access it from inside NX. There are a couple ways to do this. If you don’t need to worry about keeping your NX environment consistent across your network, then from inside NX, select the Reuse Library tab and right click somewhere in the empty space of the Reuse Library Navigator and select Library Management, then click on the Add Library button and browse to where you installed the Machinery Library. Don’t select an individual library like ANSI Inch or whatever, select the folder above the individual libraries as shown below.

If you are maintaining a consistent NX environment across your network, then you will need to use the site level customer defaults to connect to the Machinery Library. Refer to NX Network Configuration Part 1 to set up the UGII_SITE_DIR environment variable if you haven’t done this yet.

Once you have the UGII_SITE_DIR set up, open NX and go to File->Utilities->Customer Defaults and then select Gateway and then Reuse Library from the tree on the left. Make sure you have Site selected for the Defaults Level and then add the Machinery Library to the library list as shown below. Make sure you lock the library list (circled in blue).

Now everyone will be looking at the same Machinery Library. Also, if you select the Reusable Component tab, you will see a setting that allows you to establish custom naming rules and also allows you to specify where the Reusable Components are save with the are added to your assembly. This directory should be unique for each user, but should be a network folder. Using the same network drive that you used for the Machinery Library, create a folder called something like Part Family Save Directory and in that folder create a folder for each user using their logon name and then set the default to NetworkDrive\Part Family Save Directory\$USERNAME and this will work for everyone.

Using the Library

Using the library is very straightforward. You simply drill down in the library to find the component that you want and then drag it onto the design surface and when you let it go, the Add Reusable Component dialog will open allowing you to select the component size. The component that I chose below only has the inner diameter as a selectable parameter – all of the other dimensions are controlled by a spreadsheet based on the inner diameter.

So a couple things to go over with the Add Reusable Component Dialog. The first is the Placement section and the Positioning Options which are explained below:

  • By Constraints opens the constraints dialog just as if the Reusable Component were a standard assembly component – the only difference, there are Remembered Constraints in the Reusable Component that NX will ask you to define first and then from there, you can define any additional constraints. If you select Use Inferred Constraints, then NX will try to define the Remembered Constraints for you based on the face that face that you select when you drag the Reusable Component into your assembly. For example if you drag a bolt or screw into your assembly and select the cylindrical face of a hole, NX will align the fastener with the hole and touch the top face of the hole to the fastener head (there is also the option to create a component pattern when you select a hole and this will place a fastener in all of the related holes).
  • Inferred Only is more or less the same as using Constraints and selecting Use Inferred Constraints.
  • Absolute Origin and Select Origin are fairly straightforward.
  • Move will place the component wherever you let it go and then open the Move Component dialog with the Reusable Component selected.

The next section is the Pocket section. This allows you to automatically create a pocket for the Reusable Component on the other components in your assembly. If you click the Edit Pocket button, you’ll see the dialog below.

This dialog allow you to select which Reusable Components you want to create pockets for and which components you want to create the pockets in. If you are placing fasteners, the pockets will have different diameters and may have threads based on the associated section of the fastener. The pockets are created by using linked bodies and they update if the Reusable Components move or change size and you can remove the pockets after you create them.

And that brings us to Edit Reusable Component. At any time, you can right click the Reusable Component in the Assembly Navigator or the graphics window and select Edit Reusable Component to reopen the Edit Reusable Component dialog and select a different component size or edit, add or remove the pockets.

You can add your own parts to the Machinery Library, but what I would recommend instead is creating your own library and keeping your reusable parts separate from the Machinery Library and I’ll go over how to create your own reusable components in a future article. One thing I do want to go over here is how to add additional sizes to existing parts in the Machinery Library. If you open up the library folders, you’ll see three types of files, NX files, bitmaps and .krx files. The NX files are obviously the reusable parts, the bitmaps are the legends that you see in the dialogs and the .krx files are used to configure the dialogs. If you want to add an additional size to an existing part, just open it up in NX and go to Tools->Part Families and click on Edit under Part Family Spreadsheet and this will open Excel and allow you to add additional sizes.

That’s it for the Machinery Library. Hope you learned something.

Dave Holland