Download the annotated text guide with pictures or follow along with the video below.

• Start by creating a NEW part file using a Metric Part template.
• Select the Line command and lock to the (x,y plane) by pressing F3 when the plane highlights under the cursor.
  • Press CTRL+H to orient to the sketch view.
  • Click on the origin as the start point and then press “S” to create a Symmetric line about the origin point.
  • Sketch a Horizontal Line that is 50 mm long.
• Select the Symmetric Offset command found on the drop-down menu under the Offset command.
  • Set the width to 9 mm and toggle on Offset Arc in the Symmetric Offset options
  • Select the horizontal line to offset “from” and click the green checkmark or right click to accept.
• Press CTRL+I to orient to an isometric view
• Select the region created by the sketch and click an arrow to begin extruding into a 3D feature.
  • Tap “Shift” to extrude symmetrically and key-in 9.5 mm for the height.
• From the PathFinder, expand the Base Reference Planes entry and toggle on the Top Ref. Plane.
• Select the Circle by Center Point command and lock to the Top plane.
  • Press CTRL+H to orient to the sketch view.
  • Sketch a circle that is concentric with the arc and the same diameter as the arc.
• Press CTRL+I to orient to an isometric view
• Select the Extrude command from the Command Ribbon.
  • Change the selection option to “Single” in the QuickBar.
  • Be sure the option is set to ADD material
  • Select the circle and extrude symmetrically 12.5 mm
• Select the Circle by Center Point command and lock to the Top plane once again.
  • Press CTRL+H to orient to the sketch view.
  • Sketch five 4.25 mm circles as shown.
• One at each end; one in the center; tw * offset from the center
• Press CTRL+I to orient to an isometric view
• Select the Extrude command from the Command Ribbon.
  • Set the selection option to “Single” in the QuickBar.
  • Be sure the option is set to SUBTRACT material
  • Select the circles and extrude symmetrically through the part.
• Hide the PMI dimensions, Ref. Plane and Sketches by unchecking those entries in PathFinder.
• Select the Project to Sketch command from the Home tab.
  • Lock to the top face of the part for the Sketch Plane
  • Select the option to Project with Offset and click OK
  • Set the distance to offset as 1.5 mm
  • Select each of the 4 circles on that face and offset each one to the outside.
  • Change the Select option in the Quickbar to “Single Face” and offset the face edges to the inside.
• Select the 4 regions resulting from the intersecting sketches.
  • After selecting the first region, press the spacebar to multi-select the other 3 regions.
  • Select the arrow and drag into the part 4 mm to create blind pockets.
• Tap the “Shift” to toggle off symmetric cut
  • Hide the sketches and PMI dimensions from PathFinder.
  • Show the Top Ref. Plane once again
• From the PathFinder, select the last Cutout feature.
• Select the Mirror command.
  • Select the Top Ref. plane as the Mirror Plane
  • Press Esc to exit the select set
  • Hide the Top Ref. Plane
• Double click the Material entry in PathFinder to open
  the Material Table.
  • Expand Non-Metals > Plastics
  • Select ABS Plastic, high impact
  • Click Apply to Model
• Close and Save the model as CLAW LINKAGE.par in the ../ROBOT CLAW/Library folder.

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Download the annotated text guide with pictures or follow along with the video below.

• Start by opening the Claw Assembly.asm from the ROBOT CLAW folder.
• Expand the Parts Library from the fly-out menus.
  • Navigate to ..\ROBOT CLAW\Library folder
• Select the CLAW LINKAGE part you just completed modeling.
  • Place your cursor in the Preview window at the bottom of the Parts Library and rotate the preview by pressing and holding the middle mouse button (wheel) and dragging.
  • Orient the part close to the orientation it will be in the assembly.
  • This orientation will be remembered when you drag the part into the assembly and will be easier to assemble.
• The default assembly relationship is FlashFit.
  • If the first face selected is a planar face, the relationship created will be a mate or planar alignment.
  • If the first face selected is a cylinder, the relationship created will be an axial alignment.
  • Select the bottom face of the stepped area of the CLAW LINKAGE part and mate to the top face of the bottom plate of the Gripper Assembly.
  • Select the hole in the stepped end of the CLAW LINKAGE and align to the Pin in the end of the Gripper Assembly
• In the Parts Library, select the CLAW LINKAGE part again.
  • Place your cursor in the Preview window at the bottom of the Parts Library and rotate the preview to orient the part for the other side.
  • Repeat the same steps described above to assemble it into position.
• Next, find the FLAT CLAMP JAW in the Parts Library and orient the preview for assembly as the previous parts.
  • Drag in the JAW part.
  • Mate the face of the JAW slot to the bottom of the LINKAGE part.
  • Next align the two holes in the JAW to the 2 end holes of the LINKAGE parts.
• Repeat the previous steps to add a jaw to the other side.
• From the Parts Library, drag the CLAMP-PIN-LONG.par into the graphics area.
  • Press ESC before adding any relationships.
• Drag in CLAW-SNAP.par and assemble to the groove in the bottom of the pin.
  • Aligning a circular edge to a circular edge with FlashFit will automatically create a planar alignment and a cylindrical alignment in one step.
• Now let’s create a NEW subassembly of the CLAW-PIN-LONG and CLAW-SNAP.
  • Select both parts graphically, or from the PathFinder, and select the Transfer command.
  • Highlight the top assembly and select the New Assembly button.
  • Point to the Library folder as the save location and name the new assembly: LONG PIN ASSEMBLY.
  • Click OK to dismiss the Transfer dialog.
• Now that we have a subassembly we need to assemble it in place.
  • First we need to remove the Ground relationship that is added when the subassembly was created with Transfer.
  • Select the LONG PIN ASSEMBLY in PathFinder and in the bottom pane of the PathFinder select the Ground relationship and press the delete key.
  • With the Pin assembly still selected, click the Assemble command.
  • Pick the bottom edge of the head of the pin. This may require using QuickPick to get the correct edge.
  • Select the top edge of a hole in the FLAT CLAMP JAW.
• This adds a mate and an axial alignment.
• We need to place 3 more Pin assemblies, so let’s capture the relationships in the Pin subassembly to use for the other locations.
  • Select the LONG PIN ASSEMBLY in PathFinder.
  • Select Capture Fit command from the Assemble collector.
  • Click OK to learn the relationships.
• From the Pathfinder, Select the LONG PIN ASSEMBLY and drag another copy into the graphics window.
  • Note the bottom face of the pin highlights for the Mate relationship.
  • Select the top face of the FLAT CLAMP JAW as the target for the mate.
  • Next a cylinder in the Pin highlights for the axial alignment.
  • Select the other hole in the FLAT CLAMP JAW as the target for the alignment.
• Drag in 2 more Pin Assemblies from the PathFinder and select the target faces and holes on the other FLAT CLAMP JAW part for each.
• Notice that in the PathFinder, near the top, that the two CLAW GEAR LINKAGE parts are grounded.
  • You can tell this because of the blue box in the corner of the icons.
  • Select each one and delete the Ground relationship in the bottom pane of the PathFinder.
• Select the Drag command and graphically select the jaw closest to you.
  • Hold down the left mouse and begin to drag to see the motion of the jaw.
  • Note only one jaw is moving
  • Click Reset in the Quickbar and escape the command.
• We need to add a Gear relationship between the two CLAW GEAR LINKAGE parts.
• Click the Assemble command and change the relationship type to Gear from the drop down.
  • Select a cylindrical face of one of the CLAW GEAR LINKAGE parts to select its centerline.
  • Select the corresponding face on the other CLAW GEAR LINKAGE parts to pick up its centerline.
  • Be sure the Green arrows are showing the rotation in opposite directions.
  • If they show the same direction, click the Flip button at the end of the QuickBar.
  • The gears are the same size and number of teeth, so the ratio can be left at 1:1.
  • Click OK to complete the creation of the Gear relationship.
• Select the Drag command again and graphically select either jaw.
  • Hold down the left mouse and begin to drag to see the motion of the meshing gears and the realistic movement of the jaws.
  • NOTE – the limit of the jaw’s motion is due to a predefined Path relationship to a sketch defining the limits of the jaw.
• Save your assembly.

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.

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