Making a Paper Clip using 'Fit Spline' in SolidWorks

Jitesh Saini

14 Apr, 2020 07:38 PM

This tutorial aims towards creating a simple & smooth CAD Model of 'Paper Clip' (with bend) as used in stationary using help of SolidWorks.

Main learning point in this tutorial will be use of "Fit Splines" in achieving smooth sweep, this I discovered when I was learning for SolidWorks certification.

Thank you! Hope you find this helpful. :)

1. Step 1: Open a New Part file

   Start by launching SolidWorks, of-course, if not already launched and open a New Part document from Menu on Top-Left or using keyboard shortcut : Ctrl + N

   
   

   

   
   

   Here's the video of the process:

   
   

2. Step 2: Select the primary plane

   After the new part document opens up in SolidWorks Graphics window. Choose a primary plane on which you will be creating a basic sketch (say: Top Plane).

   
   

   

3. Step 3: Create the base-sketch on primary plane

   • Start the sketch in the selected primary-plane (can be done by pressing Sketch-Icon in breadcrumbs)
   • The required geometry can be obtained using combination of commands or techniques.
   • In accompanying video, various sketch tools like: lines, arcs, trim tools were used. Now, I know one of the smartest way is by activating line tool and using it to complete the basic sketch.

   
   

   NOTE: Line tool can actually adapt to different types of arcs without even going over the ribbon to select Arc tool. This is achieved by taking the mouse-cursor back to the starting-point of the line (this is not applicable on the very first line that is created). Try it for yourself, if you don;t know already!

   
   

   

4. Step 4: Add relations & then dimensions to Fully Define the sketch

   The order is important guys. I learned that after quite sometime. It is actually helpful and saves us creating a mess out of a neat sketch, which is last thing you want to deal with.

   • Add relations first. This will ensure that, sketch retains it's shape and behaves well later on.
   • Now add the dimensions (this tutorial just uses some random dimensions). If things run here & there, just drag them to appropriate places.
   • This will make sketch Fully Defined. (if you are new to CAD, note that defining the sketch fully is always a good practice for an engineer.)

   
   

   

   
   

   After this, one can simply use Sweep command to create a basic paper clip. But we will move on to add the bend in one of the loops.

   
   

   Bend actually, helps Paper Clip to clip on-to pages easily, without mutilating them.

5. Step 5: Preparing for the 'Bend' part

   Now, in the same sketch (or you can go for a new sketch), we will create a construction line as shown and define it, as needed. (shown in blue)

   

   
   

   EDIT: We need to use Split Entities command, in order to split the loop as shown below. Points in the red-circle are defined after activating the Split Entities command, and this splits the loop (in blue).

   
   

   

   
   

   Exit the sketch.

6. Step 6: Creating a Reference Plane at angle, for bent-portion of sketch

   Go to Features > Reference Geometry > Plane

   

   
   

   As soon as we activate the Plane command. We will see it's property manager on left-side. Adjacent to it will be, Fly-Out Feature Manager Design Tree (FMDT), expand it.

   In Plane property manager tab:

   • Select, Top-Plane as First Reference.
   • For the Second Reference, select the construction-line as shown.

   

   
   

   Now, we just need to define the angle w.r.t. First Reference (this step could also be done right after selecting the First Reference in this case). This will Fully Define the plane, indicated by the green message indicator as shown below.

   

   This way we have defined the plane on which bent portion will be created.

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   What we did above in Plane command?

   We told the software that we need a plane which should be at an angle to the First Reference : Top-Plane & also must pass through/contain the construction-line we used as Second Reference.

7. Step 7: Creating Sketch in Reference Plane (Bent Portion)

   In the newly created reference plane, Step 6, we will now create a sketch of the bent portion. This sketch can be created using sketch tools, or simply by using Convert Entities tool.

   Select the portion of sketch to be converted/projected from the sketch from Top-Plane, created in Step 3 (shown in blue).

   

   
   

   Now, just click Convert Entities and sketch will be created in-context from selected sketch (shown below)

   

   Exit the Sketch.

8. Step 8: Use 'Fit Spline' to get smooth & continuous curve

   Before, we can use Fit Spline, we need to initiate a 3D-Sketch.

   Go to: Sketch tab > Sketch > 3D Sketch

   Select the entities to form continuous loop in the 3D-Sketch (as shown below, in blue)

   

   Click Convert Entities. We will now obtain in-context(on edge) entities in this 3D sketch. Now, we just need to convert these entities into single & smooth curve.

   
   

   Type Fit Spline in command bar, or search otherwise for it. Press Enter.

   
   

   • Uncheck the Closed Spline option in Fit Spline property manager, if checked.
   • Adjust the tolerance & other properties as needed.

   
   

   

   
   

   Click OK. Now, we have got a smooth & single curve in this 3D-sketch, to use sweep command on this.

9. Step 9: Sweep the profile on the 3d-sketch

   Go to : Features > Swept Boss/Base.

   Choose Circular profile, or as needed. Select the 3D-sketch as Path & input diameter value. Click OK.

   

   
   

   
   

   We have got out Paper Clip (with bend). The tutorial is now complete for the time-being. Here's the result with RealView Graphics & few other View Settings set to ON.

   

   
   

   You can adjust the dimensions, or completely change the shape and maybe get this 3D printed.

   Thank you for going through this. Hope this helped you, at-least a bit. :)