How to create spur gear in Siemens NX?

Tutorial by Hegedűs György

This tutorial presents the modeling of an external spur gear in Siemens NX.
The detailed modeling process is demonstrated on this video:


UPDATE: At ~ 2:40 leave the Limit options at default (At Point). See the errata video for the reason:

  1. Step 1:

    Copy these parameters into a text file and save it. Rename the file extension to .exp.

    [degrees]alpha=20 //Reference Pressure Angle
    c=sqrt(1/(cos(alpha))^2-1)/pi() //Parameter of Involute Curve
    [mm]m=3.5 //Module
    [degrees]phi=arctan(yc/zc)+90/z //Rotation angle
    [mm]r=m*z/2 //Reference Radius
    [mm]ra=r+m //Tip Radius
    [mm]rb=r*cos(alpha) //Base Radius
    [mm]rc=m*.38 //Tooth Blend Radius
    [mm]rf=if(m>1.25)(r-1.25*m)else(r-1.4*m) //Root Radius
    t=0 //NX Parameter
    [mm]xt=0 //x Coordinates of Involute
    yt=rb*(sin(deg(t*pi()))-cos(deg(t*pi()))*t*pi()) //y Coordinates of Involute
    (Integer) z=25 //Number of Teeth
    zt=rb*(cos(deg(t*pi()))+sin(deg(t*pi()))*t*pi()) //z Coordinates of Involute

  2. Step 2:

    Launch NX, create a new model file, push the CTRL+E keys and imports the expressions.

  3. Step 3:

    Create the involute curve by Law Curve command.

  4. Step 4:

    Create a circular pattern on the involute curve.

  5. Step 5:

    Draw a line which starts from the end point of involute and tangents the curve. Set its limit by equation.

  6. Step 6:

    Launch the Join Curve command and join the line and the involute curve.

  7. Step 7:

    Draw the tip and root circles by full circle. Draw a tangent circle for the tooth blend.

  8. Step 8:

    Trim the unnecessary parts of the curves.

  9. Step 9:

    Mirror the involute curve and the tangent circle.

  10. Step 10:

    Trim the tip and root circles.

  11. Step 11:

    Create a circular pattern, set the parameters.

  12. Step 12:

    Extrude the curves to get the spur gear body.


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