3D CAD Tutorial: Robot Claw

Tutorial

3D CAD Tutorial: Robot Claw

This tutorial instructs users to create a 3D assembly with moving gears, components, and restrictions to create an articulated mechanical claw.

Level:
High School, College
Difficulty:
Advanced

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 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.

Previous Next

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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