Dial Face Mold Design

The dial face is a complex part with many raised and cut features. The finger holes cut through a spline surface, while the small spring holes meet a cutout half-way through the mold. These two features caused us the most trouble in the production of the mold.

The holes in the dial need to be solid parts on the mold. One idea was to mill out the core side such that the remaining material had raised cylinders from the surface. This would have required milling a very tall feature with a very small end-mill in order to fit between the holes. Instead of doing this, we drilled holes in the core and then pressed in aluminum pins. This was easier to perform, but still required a lot of time. We had to turn down and part off 10 small ~0.434" diameter pins about 0.85" long and then press them into milled holes. After the pins were installed, they had to be turned down to match the smooth surface of the cavity mold.

The steps required to make the core mold are shown below. A .pdf of the machining steps used for both the Dial Core and Dial Cavity can be found here:

-Rough and finish turn the smooth surface and the center boss:

-Drill and mill all ejector pin holes and pin-holes, spot drill locations for small pins.

-Turn and part all pins on the lathe

-Drill, ream, and press in small (1/16" OD)dowel pins

-Press-fit large aluminum pins:

-Turn down mold with pins to match the cavity:

We then started to use the injection molding machine to make our first round of test parts. We started with the settings left on the machine for the previous run and then iterated to get closer to our final desired properties. The first part was a short shot with only 15mm of stroke:

The two sides of the mold on the BOY injection molding machine in the LMP:

Initial speed profile for injection:

Cavity mold with shims and ejector pins on the mount:

We slowly increased the shot size until the parts were complete, then increased it further to ensure that the plastic was being packed into the mold to reduce shrinkage. We did a run of about 15 parts while varying the stroke length. We found that at 22mm of stroke we could get reliable parts, but at 24 the machine couldn't full finish the stroke and would sometimes fail to enter the packing step.

Travis came back the next day to make a run of about 20 parts to be used to adjust the bearing diameter:

The parts were designed to have a 0.020" oversized bore when accounting for 2% shrinkage of the plastic. This would give us the option to remove material around the boss later to adjust the bearing fit. As predicted, the bearing was very loose and wouldn't stick into the part on the first try.

I measured 11 parts in 3 places each to get 33 values for the bearing pocket ID on the plastic parts. The average value was 0.647" ID while the bearing was 0.629"OD. However, the average value of the plastic parts doesn't clearly represent how the bearing and plastic will fit together. The parts varied significantly in ID with a standard deviation of 0.0021". This may seem small, but this means that 95% of all parts lie within +/- 0.0042" of the mean. This is a huge variation, because if the means of the ID and OD were the same, about half the parts could be 0.004" oversized, and the other half could be that much undersized.

One idea we had was to offset the mean value of the ID to be 0.004" below the bearing OD, this mean that 95% of all parts would interfere with the bearing OD, but by as much as 0.008"! 

We were very confused, but then we remembered that the injection molding machine takes a while to settle in response to a change in inputs (stroke length, temperature, pressure, etc). We measured the last 10 parts produced from the run of 20 and found a much tighter variation, with an average of 0.646" and a 95% confidence interval of +/- 0.0013" This was much closer to what was expected of injection molded tolerances. We re-machined the center boss to have a diameter of 0.630" which suggests that 95% of all new parts will still be oversized from the bearing OD. We decided not to shave off too much material because we wanted to get the fit right the first time, and if we removed too much material it would be permanently too tight.

We are planning to mold more parts this week, re-measure them, and then shave the boss down to the final value, where we think that 95% of parts will have a good press-fit with the bearing of at least 0.001" of interference.

First Yo-Yo test!

The dial, along with all of the other parts of of YoYo, not only had to be optimized for production (with injection molding settings), but had to be optimized for fit. In our YoYo this meant after we machined our molds and injected the first run of parts, we had to test it with the other injection molded (and thermoformed) components. This lead us to make a few changes on a number of our molds. While this was expected (and the molds were made large in order to account for these differences) this made the optimization phase of production much longer and more labor intensive. For example, the Finger Stop on our YoYo did not come out with the spline curve necessary to fit over the dial. Although we had finished the base mold we needed to re-machine it in order for the Finger Stop to work. 

Through this process we learned that it is very important for each part of the team with interfering components (ie. plastic press-fits and free-fits) to communicate well on part tolerance and geometry. Although we learned this is important we also think we did a good job communicating the fits for each of our parts -- we were able to catch the mis-fits (some of which were made on purpose) during the optimization phase and before production. Communicating and organizing our designs around each-other's models is something we have learned is important and will take from 2.008 into future classes and jobs.