Used with permission from
Gear Technology, April, 1999
Modeling Gears in Pro/ENGINEER
On the Q & A Page of The Gear Industry Home Page, we have had several questions about modeling gears in Pro/ENGINEER. These questions describe problems with modeling the gear geometry, especially involute profiles, helicals, spurs and other forms. For example: "I have an application that calls for a molded sector gear. I will need to create part geometry for this design. I need help in generating an involute tooth profile. Can someone help me with suggestions how to model this in Pro/ENGINEER?" and "I am trying to model gears using Pro/E and am having a hard time with it..."
With the help of Frank DeSimone, Product Line Manager for Geometry at Parametric Technology Corporation, the authors of Pro/ENGINEER, and Daniel Gratten, a gear designer and technical specialist at Meritor Automotive, we will endeavor to answer some of these questions.
The Steps Involved The first step in modeling a gear in Pro/ENGINEER is to define the involute curve. Once this is done, the gear itself, whether a spur or helical, is simply extruded from the tooth form. In Pro/ENGINEER, there are two ways to develop this involute tooth profile: You can do it mathematically or you can do it graphically.
The Mathematical Model According to DeSimone, this is where most people get into trouble. However, he says that the following steps in Pro/ENGINEER will mathematically define an involute curve. The lines preceded by a /* are embedded notations to guide the designer. The Layout mentioned is Pro/ENGINEER's version of a template.
/*This first group of relations sets Feature Parameters to layout
/*values in the Layout "gear_calc_sm.lay"
|n = num_teeth||md = 1.25/Pd|
|Pd = diametral_pitch||cp = pi/Pd|
|a = pressure_angle||ts = cp-tt|
|Dr = root_diam||fr = fillet_rad|
|ad = addendum||rlf = relief_diam|
|tt = tooth_thick||D_o = Dp+2*(ad)|
|Dp = n/Pd||r_b = .5*Dp*cos(a)|
/*This group of relations is composed of a start angle (alpha) and
/*three simultaneous equations for r, theta, and z, in cylindrical
/*coordinates.(alpha) is calculated directly from the geometry
/*defining the involute curve.
alpha = t*sqrt(D_o^2/(4*r_b^2)-1)
/*(r) is simply the changing length of a string that defines the
r = r_b*sqrt(1+alpha^2)
/*(theta) is the angle created by the changing length of r, given that
/*the line must always be held tangent to the base circle at (r_b).
theta = 180/pi*(alpha-pi/180*atan(alpha))
/*and we want the curve to stay in the same plane, so z = 0
According to DeSimone, this mathematical procedure creates a datum curve, the basis for the involute tooth profile, using an equation. It references the Layout for key parameters but, as mentioned earlier, in the absence of geometry it has to explicitly calculate alpha to give the involute a starting point. The variable t varies from 0 to 1 over the length of the curve and is used as a time variable.
The Graphical Method
What follows is the step-by-step process to create spur or helical gears graphically that was worked-out by Dan Gratten of Meritor Automotive.
The Gear Ring
This ring can be placed on any gear blank and work. Also this helical gear ring could be used on multiple gear blanks. The following describes the process used to create this helical gear ring:
1. Begin by creating datum curves that will define the attributes of the gear. Use Feature, Create, Datum, Curve. Create the four following circles as shown in Fig. 1.
Pitch Diameter (PITCH_DIA).
Minor Diameter (MINOR_DIA).
Major Diameter (MAJOR_DIA).
Set all four of these diameters to the values on your gear spec sheet.
2. Select Modify, Dim Cosmetics, Symbol to name these circles with recognizable names as shown in Fig. 1.
3. Create the Parameters:
Using: SetUp, Parameters, Create, Number. (Enter in values from your gear summary or spec sheet.)
4. Define the gear tooth itself. Begin by creating a datum curve, and define it as shown in Fig. 2. Note that it is not a true involute profile. Using this simpler method, you will obtain about a 98% accurate representation of the tooth without creating an involute.
The tooth radius is defined by a radius that has its center lying on the base circle diameter (it is aligned to the base circle diameter). The tooth thickness is defined by two points that intersect the pitch diameter and the tooth radius. The outside of the tooth edge is used from the datum curve MAJOR_DIA and the root of the tooth edge is used from the datum curve MINOR_DIA. The fillet radius at the bottom of the tooth to the root or minor diameter of the tooth is defined in Fig. 2 as sd14 & sd15 and is defined in our gear summaries as the tip radius on the hob. This is not the exact radius. The radius on the tooth will actually be greater than the tip radius on the hob, but once again we are about 98% accurate. Complete the curve by sketching lines to the center, forming a single tooth using a datum curve. Regenerate the curve and Select OK. Select Modify, Dim Cosmetics, Symbol and add names to the tooth thickness dimension (shown as sd36 in Fig. 2 and one of the tooth radius dimensions (sd18) and the tip radius (sd14). Call the tooth thickness TOOTH_THICKNESS, the tooth radius TOOTH_RADIUS and the tip radius TIP_RADIUS.
5. Write the following relations into the part:
Make sure that you have a datum axis through the center of the diameters before you begin the next step. Then do a dependent copy of this curve and translate/rotate this curve. To do this use: Select, Feature, Copy, Move, Dependent, Done, then Select the Datum Curve, Done, Translate, Crv/Edg/Axis, and Select your center axis, Select OK, enter 1.00, Select Rotate, Crv/Edg/Axis, Select your center axis, Select OK, enter 10.0 for the angle, Select Done, Move, Done and OK.
It is best to create a relation driving these 2 Dimensions at this point. Simply Select Modify and then Select the copied Curve, Find the 10 Degree and the 1.00 Dimensions and then Select Relations and Note the system name for both dimensions. Select Add from the relations menu and type in the following:
DXX=FACE_WIDTH/3 D??=2* ASIN (DXX * TAN(HELIX_ANGLE)/BASE_CIRCLE_DIA)
where D?? is the system name for the angled Dim in the copy and DXX is the system name for the depth of the copy. Regenerate your part.
6. Create three copies by patterning the copied tooth using the two dimensions mentioned above as the driving dimensions for the pattern. This will give you a smooth translation to your helical gear. You will now have something that looks like Fig. 3. Then add relations to define the pattern which sets the patterned depth and angle = the DXX and the D?? mentioned above. Regenerate your part.
7. Create a datum curve that is aligned to the center axis of the four Diameters at a length of the face width of the gear (This dimension should now be driven by a relation D??=FACE_WIDTH).
8. Create your protrusion using Advanced, Swept Blend, Select Sec, Normal to Spline. The trajectory is the straight line curve created above along the center line of the diameters. The sections are the four datum curves created and shown in Fig. 3. Simply Use Geom Tools. Use Edge, Sel Loop on all four datum curves to define your four sections. Note: Make sure that your start points are the same on all four sections.
9. You have now created a single helical tooth for your helical gear ring. This tooth should look something like Fig. 4. Next create a copy of the first tooth using Feature, Copy, Move, Dependent, Done, Select the Protrusion, Done, Rotate, Crv/Edg/Axis and Select the center line axis as your rotating axis and then Select OK and enter your angle (use 360/Number of Teeth), then Done, Move, Done, and OK. Add the relation D??=360/NUMBER_OF_TEETH (where D?? = the system name of the dimension angle just entered above). Regenerate your part.
You can now pattern the copied tooth by using Feature Pattern and then Select the copied tooth and use the angle from the previous step to drive the pattern angle and the number of instances should be your Number of Teeth-1. Add the relations:
Where D?? and P1 are the system names that are given to the dimensions generated by the pattern creation. Regenerate your part. Once you are complete you should have something similar to Fig. 5.
10. Lastly, create a coaxial hole at a blind depth of the face width of the gear to turn it into a ring see Fig. 6 (set this blind depth dimension DXX= FACE_WIDTH using a relation and set the diameter of the hole D??=MINOR_DIA-.100 using a relation). Regenerate your part. This we use so that this gear ring can be merged into any gear blank that you have developed. Add the relations to the gear part to drive all the geometry.
Automation If you desire you can automate this process for your users to simplify this process considerably. Create a Pro/Program out of this gear ring. Add to the gear ring program the information contained in Fig. 7. This can be done by selecting Program from the main menu and then Edit Design. From there simply add the information shown in Fig. 7 in between the input and end input lines. The user merely has to regenerate the gear ring. When he does, the system will prompt him to either use current values or to enter new ones. Simply select Enter, Select All, and then answer the questions that are asked. Once all the information is answered, the part regenerates and the gear is created.
It may be useful to create four such templates: A millimeter and inch version of both a right and left hand helical gear.
Once this gear ring is completed, you can then use the Advance Utilities Function to Merge it into your gear blank. The result is shown in Fig. 8. Also merged into the gear shown in Fig. 8 is an internal spline similar to the helical gear defined above. The helical gear can be converted into a spur gear simply by entering 0 for the helix angle.
Daniel Grattan is a Technical Specialist at Meritor Automotive. He can be reached at firstname.lastname@example.org.
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