This topic explains how to model a spur gear in Pro E/ Creo completely using relations. Normally the following parameters are enough to manufacture a spur gear.
1. Number of Teeth
2. Module or Diametral pitch
3. Pressure Angle
The input parameters may vary place to place i.e someone might give outer diameter and pitch diameter instead of module or Diametral pitch. All other necessary parameters like pitch circle diameter, root diameter, base circle diameter etc. are derived using standard set of gear formulas and the input parameters.
First let me go through the gear formulas for the involute spur gear. You will have to use these formulas in ProE relations/ equations. Let’s keep the below parameters as input.
The gear formulas are, Note: These are basic set of formulas. You need to consider clearance etc. for more realistic model.
Diametral_pitch = Number_of_teeth / Pitch_diameter
Base_diameter = Pitch_diameter * cos(Pressure_angle)
Whole_depth = (2.2 / Diametral_pitch) + 0.002
Root_diameter = Outer_diameter – (2 * Whole_depth)
Addendum = 1 / Diametral_pitch
Dedendum = Whole_depth – Addendum
Circular_tooth_thickness = Pi / (2 * Diametral_pitch)
I will use the above formulas exactly in Proe relation/equation for clarity purpose. You can abbreviate the parameters if you want i.e PD for pitch_diameter etc. If you have different input parameters, interrelate the formulas to get the output values. There are two cases. The base diameter may be larger than root diameter or the root diameter can be larger than the base diameter. There are some changes in modeling the two cases. Read here to know how to handle that case.
Now, Lets take the following values (inches) for this example:
Outer_Diameter = 3.25
Number_of_Teeth = 11
Pitch_Diameter = 2.75
Pressure_Angle = 14.5
Width = 1
1. Make an extrude for the gear blank. Don’t bother about the dimensions. Just give anything for now.
2. Go to Tools → Parameters from the main menu. Create the input parameters and the enter the values as shown in the image below using the add button.
3. Go to Tools → Relations from the main menu and enter the relations. Copy paste the gear formulas given above.
4. Create three circles for Outer dia, base dia and pitch dia using sketch and name them as shown below in the model tree. Give any dimension for now.
5. Now we have to relate the formulas(dimensions) to the respective sketches. To do that, see the video below. You need to regenerate to see the result. Relate the dimensions to the respective sketches (i.e Pitch_diameter parameter for Pitch_dia feature)
Note: If you open the parameters windows now, you will see some additional parameters. This is because we created new parameters through formulas/ relations.
6. Create a new coordinate system at the center of the gear blank using the datums and front face as shown in the image. Name it “GEAR_CSYS” for reference purpose. Make sure that the Z direction points outside, X horizontally and Y vertically. I recommend to create it as shown in the image (X and Y in positive direction). This coordinate will be used to create the involute curve from equation.
7. Now the involute curve has to be created. In ProE wildfire versions, go to Insert → Model datum → Curve or use the short cut button. This will open up the curve menu manager. Click on From equation and Done. Now you have to select the newly created “GEAR_CSYS” coordinate. Then select “Cartesian”. This will open the text window.
To open this in Creo, type Curve in the search box at the top right corner and select “Curve from equation” from the list.
Now paste this equation in the text window.
Base_radius = Base_diameter / 2
Angle = t*90
Cir_len = (PI * Base_radius * t ) / 2
X_PNT = Base_radius * cos(Angle)
Y_PNT = Base_radius * sin(Angle)
x = X_PNT + ( Cir_len * sin(Angle))
y = Y_PNT – ( Cir_len * cos(Angle))
z = 0
Save the text window and close. Click done. This will create the involute curve.
8. Create a sketch for circular tooth thickness at pitch diameter from the intersection point of involute curve and Pitch diameter as shown in the video.. Give any dimension for the arc length.
9. Come out of the sketcher. Double click the sketch created in step 8 and enter Circular_tooth_thickness in the arc length value. This will relate the arc length to Circular_tooth_thickness formula.
Now, Crate a new point at the center of the circular tooth thickness curve using point option. To do that, go to Insert → Model datum → Point → point. Now click the newly created curve and enter 0.5 in the input area as shown in the image.
10. Create a new datum using the point created in step 9 and the center axis of the gear as shown in the image. This will be used to mirror the involute curve.
11. Mirror the involute curve using the datum created in step 10. The model will look like this.
12. Create a extrude for a single teeth. Use the two involute curves and the outer diameter and root diameter for the sketch. Trim all other entities. Extrude the sketch to the next face.
13. Create the chamfer and radius.
14. Group the Extruded teeth, chamfer and the radius in the model tree.
15. Pattern this group using the center axis of the gear. 11 teeth (No. Of teeth) for 360 degrees.
16. Add center hole, key way cut and chamfer to the teeth side faces. That’s it we have a spur gear now.
Multiple methods can be used to model the gear. Just understand the concept. You can also do it on your own way combining the steps.
You can now change the input values from Tool → Parameters. The model will update automatically for new values. You may get regeneration failure on gear teeth profile depending on which value it was modelled at the first place. You will have to update the tooth profile to solve this. Help.
That’s all for this topic. I hope this helped you.