Using Surface Modeling to create a door handle

Asim Rashid

22 Feb, 2018 09:46 PM

In this tutorial we will create a door handle. Creo Parametric 4.0 will be used for this exercise.

1. Step 1:

   The completed part is shown below.

   

   
   

   You can notice that the handle is slim in the center but fat at the ends. This is evident in the top view shown in the figure below

   

   
   

   Open the model DOOR_HANDLE.PRT (It can be downloaded from http://caeuniversity.com/courses/surface-modeling/)

   
   

   You can see a surface on screen created by a sweep feature as shown below.

   

   
   

   
   

2. Step 2: Modify the surface

   We will redefine the Sweep feature and add relations to make it slim in center.

   
   

   Pick the “Sweep 1” in model tree and select Edit Definition .

   
   

   

   
   

   
   

   Pick Edit Section icon and sketcher will appear as shown below. 

   
   

   

   
   

   Notice that sketch consists of an ellipse. We will add relations so that the dimensions vary during the sweep operation according to our requirement.

   
   

   Pick Relations icon the Tools tab and Relations dialog box will appear.

   
   

   

   
   

   Now enter the following relations in the dialog box.

   
   

   sd7 = 4 - 1.5 * sin ( trajpar * 180 )

   
   

   sd4 = 3.5 - 1.75 * sin ( trajpar * 180 )

   
   

   The “sd7” and “sd4” are symbols assigned to the ellipse dimensions in sketcher. These symbols might be different depending upon the circumstances. The following figure elaborates clearly.

   
   

   

   
   

   
   

   Using the trajectory parameter, trajpar, in a relation for a sweep feature allows to map any function, along the Origin Trajectory. The value of trajpar changes from 0 to 1 as the section is swept along the Origin Trajectory from start to end.

   
   

   Pick OK to save changes and exit the Relations dialog box.

   
   

   Pick OK to complete the sketch.

   
   

   Pick Apply icon to save the changes and surface will appear as shown below.

   
   

   

   
   

   Now we need to close the open ends so that quilt can be converted to a solid. For this, we will merge an extruded surface with the swept surface. The extruded surface has already been created but hidden.

   
   

   So select the “Extrude 1” feature and pick Show to unhide.

   
   

   

   
   

   
   

3. Step 3: Merging the surfaces

   Now select both quilts while holding down the Ctrl key as shown below. (Tip: You can use the Quilt filter for selection or drag the pointer over the both quilts to select them.)

   
   

   
   

   

   
   

   
   

   Pick Merge icon on the Model tab to invoke Merge tool.

   
   

   Pick on the arrow to flip its direction as shown in figure below. This is necessary to keep the desired side of the quilt.

   
   

   

   
   

   

   
   

   Now the preview will appear as shown below.

   
   

   

   
   

   
   

   Pick the Apply icon or middle-click to complete the merge feature. The quilt will appear as shown below. (If it does not appear as shown below then you need to redefine the merge feature and fix it.)

   
   

   

   
   

   Notice that the joint between both quilts appears magenta which means that both surfaces have been merged into a single quilt. 

4. Step 4: Solidifying the quilt

   Now select the quilt as shown below.

   
   

   

   
   

   
   

   Pick Solidify icon on the Model tab to invoke Solidify tool.

   
   

   

   
   

   Solidify dashboard will appear as shown below.

   
   

   
   

   

   
   

   
   

   Pick Apply icon or middle-click to complete the feature. The part will appear as shown below in the wireframe mode.

   
   

   
   

   

   
   

   
   

   The black color of contours shows that now it is no more a quilt but a solid.

   
   

   Select File > Save to save the work done so far.