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Creating Part Families 

Click here to see a video for this article.

In this NX A to Z article I will explain how to use Part Families to make adjustable parts that can dragged and dropped from the Reuse Library into an assembly and then adjusted.

Modeling with Expressions

For this article, I am going to use the bracket example that is shown in the NX help files in an effort to augment the information there. So, to model my bracket, I am just going to sketch the cross-section and then extrude it and then put in the holes. The key to making Part Families is that you need to use expressions to drive the dimensions of your part, so the first step is to create the expressions. Make sure you are in Modeling and Go to Tools->Expression and type in what you see below.

Now, we need to model the bracket and connect the dimensions of the bracket to the expressions. First create a sketch and dimension it as shown below.

Finish the sketch and Extrude it as shown below.

Sketch and extrude the end radii. The 0.100 dimension is irrelevant – you just need to make sure that the line is above the end of the bracket.

The next step is to sketch the holes. There are going to be two different configurations for the holes on one leg of the bracket. There will be a configuration with one hole and a configuration with two holes. The way to set this up in the model is to use Suppress by Expression and connect the suppressed state of the holes to an expression. The hole sketches are shown below.

When all the holes are modeled and none of them are suppressed, your bracket will look like the image below.

The next step is to create the suppression expressions, so select Single Hole 2 from the Part Navigator and go to Edit->Feature->Suppress By Expression and Click OK as shown below. Then do the same thing for Double Hole.

Now if you look at the Expressions, you will see the Suppression Status expressions for the hole features. You need to set them equal to the named expressions you created earlier as shown below.

Creating Part Families

At this point, your model is ready to be converted to a Part Family, so go to Tools->Part Families and the Part Families dialog will appear. Select all of the expressions that you created from the Available Columns list and add them to the Chosen Columns list. Some of the expressions you created won’t be there because they are dependent on other expressions.

Once you have added the columns, you need to specify the Family Save Directory.  When you add a member of a part family to an assembly, a new NX file is created for that Part Family member and this is the directory where NX saves the family members each time one is added to an assembly.  NX will save one copy of each family member.  If you add a family member to your assembly that has already been created, NX just pulls it in from this directory  This should be a folder on your network if the Part Family will be used by multiple people - this will eliminate redundant copies of the family members being on everyone's computer.  You can create a folder for each family of parts, or just put them all in the same folder.  Once you have selected the columns and the Family Save Directory, click Create to create the spreadsheet (my Create button is greyed out because I already created my spreadsheet).

When you click Create, NX will open Excel and you can fill out your spreadsheet as you see below. The first row are the dimensions of the part that I modeled and I filled in the rest of the rows. I also gave each family member and part number and name (the first and second columns respectively).

From the spreadsheet you can go to the Add-Ins tab and use the Part Family drop down. The options in the drop down are defined as follows (this is a snippet from the help files, the help files have a more thorough explanation).

  • Verify Part: Lets you find out whether a family member can be successfully created with the currently defined values.
  • Apply Values: Lets you apply the currently defined values to the part.
  • Update Parts: Lets you update family members in the Family Save Directory that have already been created.
  • Create Parts: The family member whose row is selected is actually created and saved as an NX part file.
  • Save Family: Saves the spreadsheet configuration and returns you to NX.
  • Cancel: Returns you to NX without saving any changes made to the spreadsheet.

So, you can select any of the rows and click on Apply Values to see the bracket update if you want. To continue creating the Part Family, click on Save Family and you will be returned to NX and now you can save the bracket and close it.

You want to save the bracket somewhere on your network so that everyone at your company can access it and you want to add the folder with the bracket to the Reuse Library. So, create a folder somewhere on your network called Company Standard Parts or something and put a folder in there called Brackets and then put your bracket part in it as shown below.

Then use the site level defaults to add the Company Standard Parts that you just created folder to the Reuse Library for everyone. Click here to read the NX A to Z article on implementing Site level defaults. Make sure you lock the default after you edit it.

You can see the Machinery Library in the list as well. Click here for the NX A to Z article on installing the Machinery Library.

Now, click OK to save the site level defaults and then restart NX.

Once NX is up again, create a new part file, and just drag your bracket into the graphics window from the Member Select pane of the Reuse Library and the Choose Part Family dialog will appear. Select the member you want from the Matching Members list (you can also select an attribute from the Family Attributes list to search on to filter the Matching Members list) and click OK and you’re done!< br/>

If you want to add new members, just open the Bracket model, Edit the spreadsheet and save and close.

That’s is for Part Families. Have fun!

Dave Holland