Profile

NX Release: 2206

The “Profile” command is used to create curves existing from lines and arcs connected to each other in the NX sketches. The command location in NX is shown in the figure. Also, you can start the “Profile command” by using the shortcut. (Shortcut: Z)

In the new versions, the “Profile” command is hidden in the modeling application. You can make it visible on the “Home Ribbon Bar” or “Curve Ribbon Bar”.  When you start the “Profile” command in NX modeling, Nx wants you to select a plane to create a sketch on it. Then you create a profile in the created sketch.

A profile pop-up box will open after the “Profile” command starts.  The command pop-up box is divided into two groups.

1. Object Type: You can select the curve creation method as “Straight Line” or “Arc”.
2. Input Mode: You can specify the next point’s location by using the “Coordinate Mode” or “Parameter Mode”.
   1. Coordinate Mode: You can specify the curve endpoint by typing coordinate. (Coordinate preview seen near the cursor in the graphics window)
   2. Parameter Mode: You can specify the curve endpoint by typing length/angle. (length/angle preview seen near the cursor in the graphics window)

Profile Tutorial: Draw the profile as seen in the figure.

1. Create Sketch.
2. Start the “Profile” command. 
   (Line icon active in the command box)
3. Specify the first starting point to create a profile. (Point-1)
4. Specify the following points for the connected line series to point-2,3,4
5. Activate the “Arc” in the command box.
   If the arc is not tangent to point-4, move the mouse cursor several times around point-4. The arc will parallel the line at point-4.
6. Set the “Object Type” to “Line”
7. Click on point-6,7
8. Set the “Object Type” to “Arc”
9. Click on point-8 if the arc preview looks like the figure. If not, move the mouse cursor around point-7, while it seems like the figure.
10. Set the “Object Type” to “Line”
11. Click on point-9,10
12. At the end click on point-1 to create a closed profile contour.
13. Press “Esc” twice to exit the “Profile command”
    If you press “Esc” one time, the current profile command will finish and the new profile command will start. If you press the “Esc” key twice, You exit the “Profile” command completely.

Tip 1: Look at the Cue/Status line at the bottom of the graphics window when using the profile command.
When the “Profile” command is activated, the Cue/Status line shows:

• The mouse cursor coordinates in the graphics window for the first point selection.
  The next point coordinate when the input mode is set as “Coordinate Mode“.
  
• The next point distance and angle according to the previous point when the input mode is set as “Parameter Mode“.
  

Tip 2: To specify dimensions to profile curves:

1. Finish and exit the “Profile”
2. Click on the line.
3. The curve dimension will appear. Click on the dimension and set the dimension value.
4. The selected line dimension will fix.

Tip 3: If you want to set dimensions or coordinates to the profile when drawing the profile, You should set the values in the pop-up box. (The figure shows the pop-up box)

To open this pop-up box:

1. Do not move the mouse for three sec.
2. Press the “Tab” key on the keyboard to open the pop-up box.