Creating the surface model of a hand grip

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In this tutorial we will create the surface model of a hand grip. Creo Parametric 4.0 will be used for this exercise.

  1. Step 1:

    Set the working directory to the EXAMPLES folder and open the model HAND_GRIP.PRT (It can be downloaded from http://caeuniversity.com/courses/surface-modeling/)


    The model consists of four datum curves as shown below.  




  2. Step 2: Creating the surface

    Pick Sweep icon to invoke the Sweep tool.


    Pick the straight datum curve (Sketch 1) with left mouse pick to make it Origin Trajectory. (Set the view to Default Orientation to avoid any confusion)




    Now hold down the Ctrl key and pick the other three curves to add them as chains.




    The order, in which chains are selected have no effect on the sweep geometry. Only the desired Origin Trajectory should be selected first.


    Pick References tab to open the References slide-up panel and confirm that there are three chains in addition to Origin Trajectory.


    Pick 'Sweep as surface' icon  to create a surface with this sweep feature.




    Pick Edit Section icon to sketch the cross section.

    Notice that system has placed cross-hair at the start point of the Origin trajectory and also a reference to each chain. You can rotate the view to have a look at it clearly. 



    Pick Spline icon and sketch a three point spline that passes through the references for chains as shown below.



    Now create the spline tangency dimensions as shown below.



    To add spline tangency dimension at a point, click the spline, then click the geometry to which the spline tangency is to be defined and then click the endpoint where the tangency is to be defined. Then click the middle mouse button to place the dimension.


    Pick OK to complete the sketch.


    Pick Apply and Save icon to complete the feature and surface will display as shown below.



    Notice that cross-section remains aligned to the chains all along the sweep feature.

  3. Step 3: Mirroring the surface

    Now we will mirror the surface, so select it as shown below.



    While the surface geometry is selected, pick Mirror icon on the Model tab to invoke the Mirror tool.

    Select the FRONT datum as Mirror plane.

    Pick Apply and Save icon to complete the feature. Part will appear as shown below.



  4. Step 4: Merging the surfaces

    Now we will merge the surfaces together.

    So select the surfaces, shown in the figure below, while holding down the Ctrl key. (order of selection is not important)



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

    Pick Options tab and change the merge type to Join.



    Join option is used when two surfaces have a common edge. Join option is faster than Intersect option.

    Pick Apply and Save icon or middle-click to complete the merge feature.

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




Comments

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    Jasper Aaron

    nice.. check out.. mine too bro.. i did in solids using CATIA ;)

    March 1st, 2018 07:44