Creo Parametric Gear Design: Step-by-Step Guide

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Modeling

How to Model a Spur Gear in Creo (Relations Included)

Introduction

Designing parametric spur gears in Creo Parametric allows for easy modifications and reuse in different projects. This tutorial will guide you step-by-step on how to:
✅ Model a fully parametric straight-tooth spur gear
✅ Use relations to control gear dimensions (module, teeth count, pressure angle)
✅ Generate an accurate involute curve for proper tooth profile
✅ Pattern teeth automatically based on user-defined parameters

By the end, you’ll be able to copy-paste the relations and quickly generate custom gears in seconds!

Step-by-Step Guide

1. Create a New Model

  • Start a new part in Creo (File > New > Part).
  • Ensure default datum planes & coordinate system are included.

2. Add Gear Relations

  • Go to Tools > Relations and paste the following (from previous calculations):
/***** GEAR INPUTS *******************

M = 1		/* M - gear module (in mm)
alfa = 20	/* alfa - pressure angle (standard 20 degrees)
z = 20		/* z - number of teeth
xm = 0		/* xm - profile shift value (shown on drawing)
x=xm/m		/* profile shift coefficient

ha_coef = 1	/* Addendum coefficient (standard = 1)
c_coef = 0.25	/* Clearance coefficient (standard = 0.25)

/***** GEAR CALCULATION *******************

ha = ha_coef * m		/* Addendum (tooth tip height)
hf = (ha_coef + c_coef) * m 	/* Dedendum (tooth root height, including clearance)

d=z*m		/* Pitch diameter
da=m*z+(2*ha)+2*xm	/* Tip diameter
df=m*z-(2*hf)+2*xm	/* Root diameter
s=0.5*pi*m+2*x*m*tan(ALFA)	/* Tooth thickness at pitch diameter

r_inv=d/2*(cos(ALFA))	/* Base circle radius (generates involute curve)

dl=2*(m*sqrt((((ha_coef-x)/(tan(ALFA)))^2)+(((z/2)-ha_coef+x)^2)))	/* Diameter of last involute point

For more details visit: Calculation of gear dimensions

3. Sketch 4 Circles for Gear Profile

  • Create a sketch on FRONT plane.
  • Draw 4 concentric circles and assign relations:
sd0 = df (Root diameter)
sd1 = d (Pitch diameter)
sd2 = dl (Involute limit)
sd3 = da (Tip diameter)

4. Create Involute Curve (Equation-Driven)

  • Insert > Model Datum > Curve from Equation
  • Select Cartesian coordinate system.
  • Enter the involute equations:
THETA = T * 90
THETA_RAD = THETA * (PI/180)

x = (r_inv) * SIN(THETA) - (r_inv) * THETA_RAD * COS(THETA)
y = (r_inv) * COS(THETA) + (r_inv) * THETA_RAD * SIN(THETA)
z = 0

5. Trim Involute Curve to Tip Diameter (DA)

  • Use Trim tool to cut the involute at the da circle.

6. Sketch Tooth Profile

  • Create a new sketch for the tooth:
    • Use the trimmed involute as a reference.
    • Add a tooth thickness relation: sd11 = s/2 (half of tooth width).

7. Create Base Gear Body

  • Extrude the df (root diameter) circle to form the gear blank.

8. Extrude Teeth from Sketch

  • Extrude the tooth profile with the same depth as the gear body.

9. Pattern Teeth Around the Gear

  • Select the tooth extrusion → Pattern > Axis Pattern.
  • Enter number of teeth (p90 = z in relations).

10. (Optional) Add Fillets & Final Touches

  • Apply rounds at the tooth root for strength.
  • Pattern the fillets to apply to all teeth.

Final Notes

✔ Fully parametric – Change M, z, or alfa to update the gear instantly!
✔ Reusable – Save as a template for future designs.
✔ Accurate involute profile ensures proper gear meshing.

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How to Model a Spur Gearrelations

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