This grabber was used during the FTC 2020-2021 Season (Ultimate Goal)1 to pick up the “wobble goal”. At the bottom of the page you can find a link to download the SolidWorks files for it.
Our main purpose being to design and build a grabbing and holding mechanism for a one-inch-thick cylinder, we decided that the basic setup would be similar to a pair of pliers. We explored several actuation solutions, one being a direct drive with two servos, and another one, using gears and a movable parallelogram. The inspiration for the second one was the non-powered VEX Robotics ClawKit. We decided to add a servo to it, driving one of the gears. Moreover, since we also needed different shapes for the grabbing tips, we decided to fully 3D model a custom design and then to 3D print all its parts.
The first iteration was a fairly large system, shown here next to the VEX which inspired us:
The servo directly drives a large gear, through two attachment points off center, spinning for only a fraction of the full circle, and that gear moves the one of the other arm.
Then we realized that we could miniaturize it, helping with the FTC robots size constraints, and while doing that, that it could also be reinforced, since parts inside a compact design have less wiggle room.
The full 3D Simulation animation of the second, more compact variant can be seen in the video below:
and here we see it in action (affixed on a rotating metal arm through its back metal plate):
Compared to the first variant, the second one has the arms tucked in, and actually three “floors” with gears. The reason for this was that the servo size being fixed and fairly large, we didn’t have enough room for it to directly drive the gear which would open and close the claws. The road from the initial iteration to this more compact variant went through playing with cardboard cutouts, to have a better feel:
So we managed to install the gears in between (and right above) the arms, instead of next to them. The servo drives the gear from its center, as highlighted above, which in turn drives the green gear, which is fused to one of the arms, thus driving it. Finally, that arm drives the other arm, through lower small gears.
The arm gears are cut, because they don’t rotate for a full circle, and because this way the other two arms can come up close to the geared arms in the “tuck-in” position. The green gear is also cut along its arm edge, this way allowing for the intermediate floor to continue around it and ensure overall strength. Here we have a few more views from the Solidworks assembly, followed by movement snapshots.
Notice below how the straight cut edge of the green gear turns with the arm.
Among the problems we had to solve was how to solidly hold the gears in place, appropriately setting holes in the holding plates, while also holding the plates themselves, with long screws, all that while not squeezing the gears from top and bottom too hard, so as to avoid preventing them from turning altogether. To this purpose, we used small blocks, held in place with their own screws and with a side hole where the nut was slid inside, visible in the side views above. We also used small cylinders around the long screw at the front, for the same purpose. This way we could solidly tighten these long screws to hold the floor plates, through the blocks and cylinders, onto each other, having appropriately sized the blocks to leave a fraction of a mm for the gears to be able to turn. Also, the teeth height and overall size was chosen to allow enough squeezing force to be transmitted from the servo to the claws, and the claws were eventually heightened, to counteract the fairly high gravitational torque from the “wobble”, the game piece which the grabber had to hold in the air.
About Gears and Solidworks:
- Gears are designed so that the teeth of two mated gears roll on each other as the gears spin, without rubbing hard or bumping into each other. To achieve this, the teeth contours are made to follow mathematical functions computed to ensure this geometry. While it is of course possible to purchase gears in various sizes and materials, 3D-printing them allows for more flexibility and bespoke design. Solidworks in particular offers a wide array of configurable gears, which then can be exported like any other parts, ready for manufacturing.
- To design a geared mechanism in Solidworks we start by creating an assembly. Then we open the Toolbox from the Library button, and pick the standard we want gears from. Here we decided to go with ANSI metric.
In general, gears have an overall diameter and a number of teeth. To simplify design choices, the metric gears link their various geometrical parameters through a special number called module. Two metric gears can work together if and only if they have the same module. They can of course have different numbers of teeth, to allow for various angular speed ratios. Consequently, for a given module, the larger the number of teeth, the larger the gear diameter. In particular, for module 1, a metric gear with N teeth will have a diameter of N mm.- Thus, to build such a gear, after navigating in the toolbox to the ANSI metric folder, then to the power transmission subfolder, and then to the gear subfolder, we need to drag the appropriate gear into the assembly. For our purpose here the gear to drag is the internal spur gear.
Once the gear is dragged and dropped into the assembly, a configuration menu opens up on the left and we can set the module and number of teeth, as well as the thickness of the gear, and the shape and size of the central hub hole. Once everything is validated, the gear is built into the assembly as a regular Solidworks entity, automatically generated for us with the usual extrude, cut, revolve etc operations. This powerful feature has such a simple usage because in Solidworks we can set up these operations also based upon parametrized mathematical expressions.- And now comes the beauty of it all: once we are happy with the chosen piece(s) of gear, because of course this process can be repeated, to attach for instance two gears with different diameters, to each other, concentrically, the assembly can also be saved as a part (by simply picking that option from the Save As menu). In the part, the gear(s) become one body, and we can further build various axles, or eccentric small axles to move other parts, or we can even cut a part of the gear, and so on, with the full power and flexibility of Solidworks. This is the square-hole-disk-with-gear-below, directly driven by the servo, which then drives the green intermediate-floor gear (fused to the arm):
And this is the arm with the intermediate gear:
All these have been built following the above set of steps, using so-called ‘mates’ in the SolidWorks assembly, to properly align them (e.g. concentrically), then saving them as parts, and proceeding further to extrude and to cut, into the final shapes.
By clicking on GearedGrabber you can download a zip archive with the SolidWorks files and the overall assembly.