Create a fidget spinner with parts, drawings, and assemblies

Tutorial

Create a fidget spinner with parts, drawings, and assemblies

This tutorial instructs users to create a 3D model of a fidget spinner in Solid Edge. This folder includes detailed instructions, a step-by-step video, and Solid Edge part files. This 3D model can be saved as a .STL file that can then be 3D printed. 

Level:
Elementary School, Middle School
Difficulty:
Beginner

Download

Select the following link to install the free Siemens Solid Edge 3D CAD software for your classroom (www.siemens.com/plm/solid-edge-highschool).   Students can download and install their own free copy of Siemens Solid Edge. (www.siemens.com/plm/solid-edge-student).

Next

Download the text guide or follow along below.

  • Start by creating a NEW part file using a Metric Part template.
    • Before we start, navigate to the Sketching Tab and locate
      the IntelliSketch options.
    • Open the dialog and set auto-dimensioning as shown.
    • Click OK to dismiss the dialog.
  • Draw a Ø 40 mm circle on the Top plane (x,y plane) with its center at the origin point of the base coordinate system.
  • Draw a second circle Ø 30 mm above the first and be sure their centers are aligned vertically.
  • Draw a Tangent Arc starting at about the 5 o’clock position on the upper circle, Set the radius to 20 mm, and conclude tangent and connected to the bottom circle.
  • Mirror the arc to the other side about the Y vector.
  • Use the 3 regions to symmetrically extrude50 mm.
    Hint: Tap the shift key to toggle symmetry.
  • Draw a Ø 25 mm circle on the top face of the model that is centered on the larger lower cylinder.
    • Extrdue the region to subtract a hole.
  • Use the Hole command to create a General Screw Clearance for an M8 screw on center with the smaller top cylinder.Add a Smart dimension between the holes.
    • With your mouse hovering over the value dimension, scroll the middle mouse wheel and watch the geometry dynamically adjust.
    • Make the value 40.00 mm

  • Fence select the upper cylinder, clearance hole, and tangent arc
    faces and select the Circular Pattern

    • Locate the pattern origin at the center of the
      larger bottom cylinder and set the count to 3.
  • Select the hole in the original upper cylinder and synchronously drag
    toward the center of the part.

    • Ultimately adjust the 40 mm dimension to 34 mm.
  • Add 00 mm rounds (Face select option) to the top and bottom faces.
  • Assign material by double clicking on the Material entry in the PathFinder and setting it to Non-metal, Plastics, and pick ABS Plastic high impact.
  • There is no current Lime green face style, so select Styles from the View tab
    • Pick Face Styles from the Style type
    • Select Green from the Styles
    • Click the New button to create a new “Lime Green” style based on the default Green.
      • On the Faces tab
        • Click on the Diffuse color drag the H: value to .26 and the I: value to about .83.
        • Click on the Ambient color and set H: to .26 and the I: value to .57
        • Click on the Specular color and simply set H: to .26
      • Click on the Edges tab and select the option to “Copy from Faces Diffuse Color”
        • Drag the I: slider to about .35
      • From the View tab, select Part Painter
        • Set the Style to the new Lime Green
        • Set the selection option to Body
        • Select the part to make it Lime Green.
      • From the Application button, select Info and then File Properties.
        • On the Summary tab fill in the Title, Subject, Manager and Company.
        • On the Project tab, fill in the Document Number, Revision Number and Project Name
      • Save as “Spinner.par” to the Fidget Spinner

Previous Next

Download the text guide or follow along below.

  • From the Application button select the New tab and choose Assembly of Active Model.
  • Select the Parts Library from the fly-out menu and click on Bearing.par.
    • Note if you click in the drag in the preview window you can orient the part close to what you will want it to be in the assembly
      • This makes creating relationships easier and more obvious.
    • Drag Bearing.par into the graphics window.
      • FlashFit is the default assembly relationship type so simply select the center cylinder in the bearing and align with the center hole in the spinner
      • Change the relationship type to Center-Plane and be sure the option is set to “Double”.
        • First select the top and bottom planar faces of the bearing to find its center plane and then select the top and bottom planar faces of the spinner to align with its center plane.
        • Note the bearing extends equally on both sides of the spinner
      • Notice the center hole in the spinner is much too large to hold the bearing. From the Inspect tab select the Smart Measure command and select the outside edge of the bearing to gets its diameter. (22 mm)
      • Using the Select tool, pick the face of the center hole in the spinner.
        • Use the Smart Dimension value to change the 25 mm diameter to 22.4 mm diameter.
      • From the Parts Library drag in the M8x14Lng-Screw.par.
        • Select the cylinder on the screw and align with an outer hole in the spinner.
        • Mate the bottom face of the screw head to the top face of the spinner.
      • From the Parts Library drag in the M8 Nut.par.
        • Select the hole in the nut and align with the screw cylinder.
        • Mate the face of the nut to the bottom face of the spinner.
      • Select both the screw and the nut from the PathFinder in the assembly and align the center of the steering wheel with the center of the screw.
        • Choose the option to Move-Copy from the QuickBar and select the steering wheel plane to start the copy.
        • Be sure the key-point filter is set to find centers and snap to the center of one of the remaining holes and click to accept.
          • In the relationship options dialog be sure to enable “Repair unsatisfied relationships” and “Replace to other components only (where possible)”. You may also check the option to remember these settings.
          • You will need to select the Spinner part for the relationships to reconnect to the new spinner hole.
        • Repeat the same process to copy the screw and nut to the remaining hole.
      • In order to put the spinner in motion we need to reorder the parts and change which part is grounded.
      • In the PathFinder drag the Spinner.par below the Bearing.par.
      • Select the Spinner.par and delete the Ground relationship from the bottom pane of the PathFinder.
      • Select the Bearing.par and add a Ground relationship from the Assembly collector on the home tab.
      • Using the Drag command with the rotate option, select the spinner part and the center axis of the center hole and while holding down the left mouse button drag the spinner around to show its motion.
      • Select the command to add a rotational motor.
        • Notice the Tool Tip video
        • Select the Spinner part to add the motor to and the center axis to rotate about.
        • The arrows will flip the direction of rotation.
        • Click Finish to accept and note the motor is added to PathFinder.
      • Select the Simulate Motor
        • Accept the Rotational 1 motor to simulate and default settings by clicking OK.
      • Click Play on the timeline to put the Fidget Spinner Assembly in motion.
      • Close out of motion simulation.
      • From the Application button navigate to the Info tab to access the File Properties.
        • On the Summary tab add:
          • Title: Fidget Spinner Assembly
          • Subject: Toys
          • Author – your Name
          • Manager: your Manager
          • Company: your Company
        • On the Project tab add:
          • Doc Number: FS-001-ASM
          • Revision: A
          • Project Name: Fidget Spinner
        • Save the Assembly as “Fidget Spinner Assembly.asm”

Previous Next

Download the text guide or follow along below.

  • From the Application button menu select the New tab and pick the command to create a
    Drawing of Active Model

    • Use the ANSI metric draft.dft template and run the wizard.
  • Place a “Shaded with edges” isometric view on the drawing sheet.
  • Hover over the Parts List command to see the animated tool tip, then click to run the command.
    • Select the drawing view
    • In the Parts List Properties dialog, open the General tab and select the “Fidget Spinner” from the Saved settings.
      • NOTE: If you did not run the setup, you will not have this entry
    • Note the Columns, Balloon, and List Control tab settings then click OK to dismiss the setting dialog box.
  • Place the Parts List on the top of the sheet and zoom up to see the information.
  • Select the balloons to see the alignment shape.
  • Add another Balloon for the nut which is not shown in the view.
    • Size: 4.00
    • No leader
    • Upper number: 4
    • Place attached to the #3 Balloon.
  • Holding down the ALT key, select the end of the #2 arrow and drag to another edge of the spinner.
    • Drag the balloon location along the alignment shape.
  • Add another Sheet to the file.
  • Run the Drawing View wizard again and select the Spinner part.
    • Change the option to place a Top view and set the scale to 3 before placing the view.
    • Show that you can drag off other views, but don’t actually place any.
  • Add a center mark in the center hole.
  • Create a vertical cutting plane on the view as shown.
  • Create a section view and turn off the hidden lines.
  • Add Center Lines to the holes

Save the drawing file.

Previous Next

Download the text guide or follow along below.

  • From Sheet 1, double click on the drawing view of the Fidget Spinner Assembly to re-open it.
  • Select the Spinner part and edit in place
    • CTRL+Q to hide the background parts
  • Using the Project to sketch command, Lock to the top face of the spinner, and choose the option to offset.
    • Set the offset distance to 2.00 mm
    • Select the outer edge of the round of each hole and offset to the outside.
    • Using the Tangent Wireframe option select the edge of the outside round of the entire part and offset to the inside.
  • Select the region created by the offsets and drag down 1.00 mm to create a cut.
  • Select the Cut feature from the PathFinder and Mirror the feature about the Top Reference plane.
  • Run the Project to sketch command again and lock to the face of the recessed area.
    • Set the option to offset and the distance to 3.00 mm
    • Offset the edges of the center hole and one of the 3 outer holes to the outside of the embossed area.
    • Offset the outer edge of the recessed area to the inside of the part as well.
  • Select the interior region created by the offset geometry and drag a cutout through the part.
    • Delete the sketch
  • Hide the PMI dimensions
  • Select the last cutout feature and create a 3 count circular pattern about the center hole to replicate the cutout in each arm of the spinner.
  • Use the round command to break all sharp edges in the Spinner part with a .25 mm radius.
    • Use All Fillets and All Rounds selection options.
  • From the PathFinder hide the Base coordinate system and the PMI dimensions.
  • Hover over a face of the part and wait to get access to QuickPick (Right click)
    • Select the “Design body” from QuickPick
  • Drag the Steering wheel to the center line of the center hole.
  • Set the option to Move-Copy on the QuickBar.
    • Select the Torus of the steering wheel to initiate a rotation and copy the geometry at an angle of 60°.
  • Access the File Properties from the info tab of the Application button menu.
    • On the Project Tab change the Revision Number field to “B”
    • Click OK to dismiss the properties dialog.
  • Save the part file
  • From the Application button menu select 3D Print
    • Click Preview to see the part located on a print bed with overall dimensions.
    • Note the STL export options
    • Export the part as an STL or if online you can see the option to order online
  • Close and return to the assembly.
    • Note there will not be fastener in the 3 new arms that were created.
  • Select a Screw and nut pair from the PathFinder.
    • Drag the steering wheel to the centerline of the screw
    • Select the option to Move-Copy from the QuickBar
  • By selecting the plane in the steering wheel initiate a free form Move-Copy to drag a copy of the screw and nut set to one of the empty holes.
    • Select the Spinner part to re-establish an axial alignment relationship to the new hole and accept.
    • Repeat this process twice more to fill all three empty holes.
  • You can now “Simulate” the motor again to see the assembly spin on the bearing.
  • Access the File Properties from the info tab of the Application button menu.
    • On the Project Tab change the Revision Number field to “B”
    • Click OK to dismiss the properties dialog and Save the Assembly
  • Return to the drawing and note the indication that the assembly/parts have changed.
    • Update the views
    • Note the drawing view tracker
      • Select Clear All and dismiss the tracker.
    • Adjust the balloons on the Assembly drawing view.
      • Drag along the alignment shape
      • Use the ALT key to select the arrow point and move to different parts of the geometry.
    • Note the updates to the Parts list
      • Revision Number and quantities
    • On sheet 2 notice the drawing views for the spinner part have updated.
      • Edit the cutting plane if necessary to go through the entire part.
      • Add another Center line for the new hole.
    • Add the Bolt Circle center marks.
    • Create a detail view from the section view.
    • Add a few SMART dimensions as shown.
    • Save the drawing.

Congratulations! This concludes the exercise.

Don’t stop here!

Improve 3D Spatial Thinking and Creativity with more examples on the GearupU website.  Developed by a Utah State design and engineering teacher focusing on STEM to STEAM, GearupU exposes students to a world of amazing patterns, shapes and artistic designs and gets them excited about STEM.  Students with no background in 2D or 3D design should start with Class 1.

Previous

Solid Edge for Students

With Solid Edge, students have access to a free version of the same easy-to-use software suite used by professionals. In addition to free software, we provide tutorials, webinars, online courses and certification to help you develop your design and engineering skills.

Training that fits your needs

Get free access to topic-based or project-based tutorials, online self-paced courses and interactive learning resources. Training materials can be used to learn Solid Edge on your own, or to supplement classroom learning. Students can also achieve Solid Edge Certification for a competitive edge when applying to jobs.

A vibrant online and offline community

Access our online Solid Edge User Community, including a dedicated forum for students. Learning Solid Edge also gives you the opportunity to participate in a variety of projects and competitions, including the Greenpower Challenge and Siemens PLM Software Student Design Contest.

We also offer a University Edition that includes more capability for a site-wide implementation. Instructors should visit Solid Edge Resources for Educators for details.

Learners of all ages can gain valuable experience with industry-leading technology, supporting your studies in STEM subjects at all levels of education, from elementary school through university.

How would you rate this content?