Posts Tagged ‘NX CAD’


NX – Create a family of standard parts (Excel)

Wednesday, July 4th, 2012

Design Intent:  The most common use of Part Families is to define a standard library part that has many variations.

     1.  Create an hexbolt  

     2.  Rename the expression that you want to keep

             a: Width = the radius of the cap

             b: Length = length of screw

     3.  Define the columns for the Family Table.

 >Choose Tools→Part Families from the main menu bar.

 >Make sure the Importable Part Family Template option is  cleared.

 >Click OK on the Warning dialog box.

 >Select the width expression from the top window of the Part Families dialog box.

 >Click the Add Column button.

 >Select the lenght expression from the top window of the Part Families dialog box.

 >Click the Add Column button.

Note:  Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.

> Change the option menu at the top of the dialog box from Expressions to Features.

> Double-click chamfer from the top list of the Part Families dialog box.

Note:  The order in which you select the attributes determines the order of columns in the spreadsheet.

Tip:  In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.

     4.  Create the family table.

  > Click the Create button from the bottom portion of the Part Families dialog box.


 > Type in a few values

    5.  Verify a family member

 > Select a cell in row 3.

 > From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.

The NX session becomes active and the family member is displayed in the graphics window.

 > Click Resume in the Part Families dialog box.

Warning:  The Part Families dialog box may be obscured, if so, click anywhere in the NX window.

     6.  Save the Part Family and the template part.

 > From the spreadsheet menu bar, choose PartFamily→Save Family.

Note:  The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.

Note:  In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.

Since we do not use this part anywhere else we are not going to do that.

     7.  Close all parts.

NX – Modeling a tapered thread

Friday, May 4th, 2012

Currently, the NX Thread command can be used to create a fully modeled straight thread. When this command is run and the Detailed Thread type is selected a fully modeled thread will be created. NX provides Modeling tools which allow users to create fully modeled tapered threads. The Variational Sweep is one of these tools.

1. Create a Datum CSYS on the centerline of the thread at the start location of the tapered thread.

2. Create the following expressions in the Expression editor.

ANGLE will be the included angle of the thread profile. This is typically 60 degrees.

L will be the length of the thread.

P is the thread Pitch which is the distance from thread to thread.

START_DIA is the diameter at the start end of the thread.

TAPER is the taper of the thread.

END_R will be the calculated value L*TAN(TAPER)+STRT_R.

STRT_R will be calculated as START_DIA/2.

All expressions should be created as Length type expressions except for the ANGLE and TAPER variables. These two need to be set to the Angle expression type. If these variables are not created as Angle type expressions they will not be selectable when creating the feature.

3. Start the process by creating a Helix curve.


The Number of Turns will be calculated by dividing the Length by the Pitch or L/P using the defined expressions. The Pitch variable will be specified using the expression P.

4. To create the tapered helix the Radius Method Use Law will be used. When selected the Law Function window will be displayed. At this point select the Linear type.


5. Specify the Start and End radius values by supplying these expression variables.


Note that the tolerance of the helix can greatly influence the accuracy of the thread.

Initially the helix will be created to the model tolerance in effect when created. This can be found at Preferences => Modeling => Distance Tolerance.

If the accuracy needs to be improved after the helix is created a higher tolerance can be specified by editing the helix and changing the tolerance value.

6. After the helix is created select Insert => Sweep => Variational Sweep. Select the helix curve as the path. For Plane Orientation pick the Through Axis option and select the centerline of the helix for the vector. For the Sketch Orientation select the same axis.


7. When OK is pressed a Sketch will be created. At this point create the profile of the thread. Constrain all geometry to the point that was created on the helix curve when the Variational Sweep operation was started. This is an important step.


It is significant that the width of the thread be smaller than the Pitch (P-.01). If this width value is too large then the model will intersect itself as it sweeps along the helix guide curve. This would cause an invalid solid to be created.

8. When the sweep is complete a hollow thread profile will be created as seen below.


9. The thread would be completed by Uniting it to the model of the base of the thread.


This same procedure can be used to create a multi-lead thread. When creating the Variable Sweep Sketch of the thread profile create two threads at half the Pitch in width. See the sketch below along with the picture of the resultant multi-lead thread. The colors of the different leads have been altered for emphasis.

Using tools provided in NX, users can quickly and easily model complex features.

Original article courtesy of Randall Waser, Siemens.


How to add an attribute column to a BOM in NX

Tuesday, April 3rd, 2012

In the part attribute, I’ve created the Plist attribute, make sure you have the object selection set to “apply to component as part attribute” if you want to save the information in the part, otherwise use the “apply to occurrence in the assembly”.

In the part list I’ve created a new column and did a RMB on the full highlight column

Select Style and go to the column tab.

Click on the arrow.

Select Plist from list and OK twice.


How to measure a volume enclosed by assembly parts or cavity in NX.

Thursday, February 2nd, 2012

In the following assembly I need to find the volume inside the gearbox, by using SPACE FINDER from the Analysis menu.

When specifying the interior point, make sure that the point is in the space that we need to measure and not on a face. Select the part making a close environment



The space finder also create 2 datum plane specifying the minimum and maximum, this information helps us define the maximum height of volume needed using the volume-height analysis section.

 In this section you can specify either you maximum height or volume and save it has a faceted body.

This is a fast and easy way to evaluate the quantity of liquid needed, for more precise evaluation other tools are necessary.