Posted Date: 22 Jun 2012 |Updated: 22-Jun-2012 |Category: Others|Author: Jignesh K Patel|Member Level: Gold|Points: 70|
This lesson covers the development of 'involute' gears. An involute gear is based on an involute
curve, which is a mathematical shape. This article includes simple steps for generating involute curves then followed by simple extrude in Pro Engineering software. Involute curve is generated by simple equation.
This article deals with complete procedure to make involute profiled gear modeling in Pro-Engineer software. Follow the steps to get ahead.
STEP:1 Generating involute curve by an equation.
Pick File, New,then enter < involute_gear > for the name of the new part
Pick OK, in the ,New, dialog box
Pick Insert, Model Datum, Curve, From Equation, Done,
Select the default coordinate system, then pick Cartesian
In the Notepad window, enter the following equations: radius of the cylinder = 3.00 angle = t * 90 s = (3.14* radius of the cylinder * t ) / 2 Xc = radius of the cylinder * cos(angle) Yc = radius of the cylinder * sin(angle) X = Xc + ( s * sin(angle)) Y = Yc - ( s * cos(angle)) Z = 0
Pick File, Save and File, Exit in Notepad
Pick OK in the dialog box
The result is shown here
This curve will be used to create an involute gear
STEP:2 Create a Cylinder.
Select the FRONT datum plane
Pick the Extrude icon
Press and hold the right mouse button and select Define Internal Sketch
Pick Flip in the Sketch dialog box
Pick Sketch in the Sketch dialog box
Sketch a circle centred on the references, with a diameter of 6.500, to represent the Outside diameter of the gear (see the figure on the previous page)
Pick the checkmark to complete the sketch
Enter < 1.750 > for the depth then pick the checkmark in the dashboard tool
Pick View, Orientation, Standard Orientation
The result is shown below, be sure the curve is in front of the cylinder as shown
STEP:3 Create three circles representing the major diameters.
Create a circular sketch on the FRONT datum plane with a diameter of 5.376 to represent the root diameter of the gear
Create a circular sketch on the FRONT datum plane with a diameter of 5.638 to represent the base diameter of the gear
Create a circular sketch on the FRONT datum plane with a diameter of 6.000 to represent the pitch diameter of the gear
The result is shown below
STEP:4 Create a datum point a datum curve.
Set the selection filter to Datums, pick the involute curve and the 6.000 diametercircular sketch, then pick the Point icon and then pick OK to create a datum point.
Be sure the selection filter is set to Datums
Pick RIGHT, TOP, and FRONT then pick the Point icon then pick OK
Pick Insert, Model Datum, Curve, Done
Pick the two datum points then pick Done and OK
The result is shown below
STEP:5 Create a datum evaluate feature.
Pick Insert, Model Datum, Evaluate
Enter < measure > for the name of the feature
Pick Create, then enter < angle > for the name of the measurement parameter
Pick Angle, then pick the TOP datum plane and the curve you just created through the points
Pick Done then read the message window and look at the model tree
Save the part
Pick the involute curve then pick Edit, Copy
Pick Edit, Paste Special
Add the checkmark next to Apply Move/Rotate transformations to copies in the dialog box then pick OK
Pick Rotate in the right mouse button popup menu
Pick the axis in the center of the cylinder then enter < -30 > for the rotation angle
Pick the checkmark in the dashboard tool
The result is shown
Double pick the copied involute curve
Double pick the 30 dimension
In the small text box, carefully enter: angle: FID_MEASURE + ( 7.5 / 2 )
Pick Yes to add the relation
Pick Edit, Regenerate
The result is shown
STEP:6 Mirror the copied involute curve.
Pick the copied involute curve (the one created in task 7) then pick Edit, Mirror
Pick the TOP datum plane then pick the checkmark in the dashboard tool
The result is shown
STEP:7 Copy the curve again.
Pick the copied involute curve then pick Edit, Copy Pick Edit, Paste Special
Add the checkmark next to Apply Move/Rotate transformations to copies in the dialog box then pick OK
Pick Rotate in the right mouse button popup menu
Pick the axis in the center of the cylinder then enter < -15 > for the rotation angle
Pick the checkmark in the dashboard tool
The result is shown
STEP:8 Copy the curve again.
Pick the copied involute curve then pick Edit, Copy Pick Edit, Paste Special
Add the checkmark next to Apply Move/Rotate transformations to copies in the dialog box then pick OK
Pick Rotate in the right mouse button popup menu
Pick the axis in the center of the cylinder then enter < -15 > for the rotation angle
Pick the checkmark in the dashboard tool
Create an extruded (through all) cut using the edges of the curves as shown below Trim the sketch as shown below.
STEP:9 Pattern the cut.
Set the selection filter to Features then pick the cut you just created
Pick Edit, Pattern, then set the type of pattern to Axis in the dashboard tool
Select the axis in the center of the cylinder
Enter < 24 > for the number of instances in the pattern
Pick the checkmark in the dashboard tool to complete the pattern
STEP:10 Finish the part.
Create a 0.020 round at the base of the gear tooth
I am using Pro E Wildfire 5. I cannot find the evaluate feature, refer step five. Is there any other way around it?
Guest Author: Mark H22 Oct 2013
Regarding this example, where did you ever refer to Base Diameter circle that is required to create the involute curve? Why apply a rotation angle of -30 degrees when the resulting curve/geometry is never shown on your screen shots?
I am using Pro E Wildfire 5. I cannot find the evaluate feature, refer step five. Is there any other way around it?