Take a look at our final presentation! And our army of minions! The story of our team this semester was definitely about mold making. We made 24 molds in all and learned a lot about the perils of curved parting surfaces. Throughout the course of the spring we also learned how to machine our molds much faster by significantly increasing the feed rate during finishing toolpaths (2-4x faster than pre-set values in Fusion). Because all of our finishing passes had a tiny stepover of 0.002″, the material removal rate (and therefore the cutting force) was small and so we were able to justify increasing the feed rate so that the MRR was comparable to other toolpaths that were removing more material at a time. Increasing the feed rate typically cut machining time by 70% so our team reaped hours of time-savings which was critical since we had to remake our molds many times! Watch out for our 50 minions yo-yoing around campus 🙂

This week, we’ve had some issues with the critical dimensions of our 3 injection molded parts, leading to us re-machining multiple molds.

Injection Molding

Yellow Face

In injection molding this part, we continued to run into the issue of the part not successfully ejecting from the mold. We tried a few “quick” mold fixes, including increasing the size of the sprue hole to eliminate any chance for undercut like we experienced in the past, applying mold release, and tapping more threads into the core side sprue hole. These worked with varying success (from no success to zero success).

Further analysis led to the realization that plastic was shrinking and holding tight onto the mouth and hair features on the cavity side of the mold. There isn’t technically an undercut on that side of the mold, as that would be impossible to machine, but the extrusion for the feature gets sheared forward and creates more of an undercut as the clamp force pushes the mold parts together and creates the shutoff area. To avoid this entirely, we’ve put the features on the core side of the mold. This way, if plastic does grab onto the feature, the ejector pins will take care of it sticking. This will also just give us a better surface finish overall, as the milling operations necessary will not have to work around the extruded hair and mouth features.

For this part, the plan from the beginning was to re-machine the other two molds (goggle and blue base), should the critical dimensions of the parts need to be changed due to the huge disparity in machining time between the blue base and the goggle molds versus the yellow face. Aside from moving the features over, the two critical dimensions of the outer snap that interfaces with the blue base, and the upper snap with the goggle will not be altered.

Goggle

Since last week, we have re-machined the goggle mold to remove the accidental partial hole in the mold cavity. We were able to successfully machine a new part, but this led to another, very unexpected issue.

The new goggle mold fixed some of the issues we had in the previous mold. We were able to successfully eject the parts due to increasing the size of the sprue hole on the cavity side to eliminate any undercut that may be created there.

However, the parting plane between the 2 mold surfaces was not entirely flush, so the shutoff that was supposed to be created when the molds were engaged leaked plastic through. Therefore, there was quite a bit of flash involved in any parts we tried to injection mold. This presented a host of defects that couldn’t be fixed with changes to the parameters in the injection molding machine. We aren’t sure why this happened, but we will look at the CAM again to see what went wrong on our end.

On the bright side, the goggle inner diameter snaps decently well with the yellow face mold. This critical dimension is fairly solid, but we would like a tighter snap between the two parts, so when we re-machine the goggle to fix the shutoff surfaces, we will be slightly decreasing the goggle’s inner diameter.

Blue Base

The blue base has given us the least amount of issues, as expected. For this part, we still need to machine the shoulder bolts, and finalize its snap dimension. It’s snapping diameter is too large for the yellow face to accommodate it. We will be shrinking this diameter down in our next iteration of the blue mold. We don’t expect other issues with this part.

Thermoforming

Mouth and Hair

The mouth and hair die gave us a few issues on the 3D printer, but that was because of a failed “join” between bodies in Fusion. We filled the hollow inside of the part in the CAD, but it created a new body which wasn’t selected anytime we sent the .stl file to the printer. After figuring this out, we were able to thermoform some trials of the hair and mouth features.

We are going to continue to work on the way this die interfaces with the yellow face and the blue body, which are hopefully finalized within the week.

Clear Dome

There isn’t too much going on with this guy (which is honestly really nice because oh boy). We’ve thermoformed a bunch of these parts, and have punched them with the white plastic used for the sclera. We are looking to get all of the domes we need thermoformed and punched while we work through other obstacles with the more complicated injection molding parts so this doesn’t have to be done as we near the end of the semester.

A. Blue Body

The blue body is our simplest part so it was the easiest and quickest mold to make. The core side took 29 minutes to machine and the cavity side took only 5 minutes to machine. The toolpaths for the mold halves were as follows:

These are the toolpath operations for the blue body mold core and cavity. Both toolpaths begin with center drilling, then deep drilling of either the ejector pin holes or shoulder bolt hole, followed by facing the top of the stock to create a uniform and smooth model top. Next adaptive toolpaths are used as a roughing pass to clear material into the general shape of the mold before finally a finishing toolpath with a smaller vertical and horizontal stepover is used to create a smoother surface finish.

We choose to use 5000 RPM for the spindle speed for every operation because that is the maximum speed of the milling machine. Since the machining time was short for these mold halves with the default feed rates, we used the pre-set feed rate values for all of the operations. In practice we would often slow down the feed rate to 30-40% of the programmed value when just starting an operation to make sure the toolpath was doing what we expected it to do before ramping up to 100% of the programmed feed rate. We were successfully able to machine this blue body mold on our first attempt.

Successfully machined blue body mold core and cavity

B. Yellow Face

Amongst the injection molded parts in our yoyo design, the yellow face is a complex piece due to the small features of hair and mouth elements in the design. In terms of machining, the core side of the yellow mold was straightforward, and very similar in toolpath to the LMP yoyo mold, taking a total of 1 hour 21 minutes to machine. The cavity side, on the other hand, required a total of 6 hours and 14 minutes of machining. Due to the long machining time, it was necessary to run the first four toolpath operations, as illustrated in figure 5, on the ProtoTRAK mill, and leave the remaining finishing operations to be run overnight on the HAAS.

Toolpath operations for the yellow body core and cavity molds. The core toolpath begins with centre drilling followed by a deeper drilling operation for ejector pin holes. Both cavity and mold toolpaths include a facing operation of the stock top to create a smooth top surface. Facing is followed by adaptive passes to remove as much material possible. On the cavity mold, a contour operation is run to remove the majority of material on the hair and mouth features prior to transporting the mold to the HAAS. This contour operation is important to carry out in order to prevent the endmill from breaking on the HAAS. On the HAAS,  the finishing scallop (0.002” stepover) and pencil toolpaths are used to reach material between small features, and create a smooth surface finish.

We chose to use 5000 RPM for the spindle speed for every operation because that is the maximum speed of the ProtoTRAK milling machine. The only exception is the spindle speed set for the scallop operation for the cavity mold, which was set to 7500 as it was carried out on the HAAS to speed up the operation. Since the machining time was relatively short for the core mold, we used the pre-set feed rate values for all of its operations. Again, for the scallop operation of the cavity mold, along with the spindle speed change, the feed per tooth was set to 0.00075 in– much smaller than the default value, to get a better surface finish in a shorter time interval. In practice, we would often slow down the feed rate to 30-40% of the programmed value when just starting an operation to make sure the toolpath was doing what we expected it to do before ramping up to 100% of the programmed feed rate. We were able to machine two iterations of the yellow cavity mold. The first mold iteration did not result in favorable outcomes due to errors in machining and choice of tools. The order of operations on the first core mold was incorrect as the 5° drafting tool had to plunge into a pocket of material rather than simply drafting a vertical surface once all material was cleared. Additionally the toolpath created for the overnight HAAS operation on the cavity did not leave a smooth surface finish and messed up the parting surface of the part by removing material along the perimeter so the part was no longer circular or flush. In our second iteration, the mold was placed on the HAAS, however, after the job was initiated, the 1/16th endmill used for the scallop operation broke when trying to remove material from around the mouth and hair features. This was because endmill attempted to remove large chunks of material around the very narrow areas of the mouth and hair. We revisited our design, and introduced a contour operation on the ProtoTRAK preceding the scallop operation on the HAAS, which removes as much material possible around the two small features of the hair and mouth. Even though the surface finish is poor on our second attempt, the mold halves successfully fit together so we were able to try to injection mold.

Two attempts at the yellow face mold. Our first attempt on the left has order of operation errors on the core and toolpath errors on the cavity. Our second attempt successfully made the yellow face core however the cavity side surface finish is poor due to the tool breaking during the overnight HAAS operation.

C. Goggle

The goggle mold went through many iterations before we were able to successfully machine both halves of the mold so that they fit together. The first iteration attempted to use traditional flat parting and shut off surfaces which caused the halves of the mold to wedge when they came together. If there was even a tiny amount of misalignment the mold halves would not fit together, causing us to pivot and pursue curved parting surfaces.  In our second machining attempt the surface finish on the cavity side finished poorly despite having a 0.004” stepover. It appeared the adaptive roughing toolpath went too deep and removed too much material. After further investigation we discovered the tool height of the endmill we used for that roughing operation was off by 0.060”. In addition to this, the two halves of the mold did not fit together and there was a horizontal offset between the mold halves so that the sprue hole did not align. We tried to investigate this offset further however all critical dimensions matched the CAD model leading us to guess that we may have incorrectly zeroed the x/y coordinates of the machine or that the stock could have been slightly off. On our third attempt we were finally able to successfully machine both halves of the goggle mold using the lessons we learned in the earlier attempts including using a curved parting plane with a steepest angle of 10° which worked better than a drafted parting plane since the curved surface is symmetric. We also decreased the stepover on the finishing operations to 0.002” to ensure the parting surfaces would close completely to shut off all plastic.

Furthest to the left is our first unsuccessful attempt at the goggle mold. The vertical shut off surface caused the mold halves to wedge together instead of closing fully. In the middle is our second unsuccessful attempt at the goggle mold. The surface finish on the cavity side is poor due to an incorrect tool height which caused the roughing operation to remove too much material. Furthest to the right is our successful goggle mold. There is a curved parting plane so the mold halves close together smoothly. Additionally, a 0.002” stepover was used on the finishing pass on both molds so that the shut off surfaces fit together tightly when the mold is closed.

The core side took 1 hour to machine and the cavity side took 1 hour 40 minutes  to machine. The toolpaths for the mold halves were as follows:

We used 5000 RPM for the spindle speed for every operation because that is the maximum speed of the milling machine. We also always used the largest tool that could fit into and cut the necessary areas in order to reduce machining time. For most operations in these toolpaths we used the pre-set feed rate values, however, we did significantly increase the feed rate of the scallop finishing pass on the goggle cavity because this operation was the rate limiting step and it was only removing 0.002” of material. We choose the scallop operation as the finishing pass because it creates passes at a constant distance from another by offsetting them inwards along the surface rather than only doing either a horizontal or vertical stepover. For this operation on the cavity a ⅛ inch ball end mill was used because it was the largest tool that could fit in all of the grooves and the cutting feed rate was changed from the default 15.3 in/min. to be 52.5 in/min. The feed rate was increased in order to reduce the time of this operation from 4.6 hours to 1.3 hours. The material removal rate (MRR) was relatively small due to a very small stepover of 0.002” chosen to create an extremely smooth surface finish. Since the MRR was small, the cutting force was small, hence, we were able to increase the feed rate. We also increased the feed rate of the ramp operation on the core side from 50 in/min to 70 in/min and we increased the scallop operation on the core side from 90 in/min to 120 in/min because these operations were similarly removing a small amount of material so the cutting force was small and allowed us to speed up the feed rate. Since we were not able to get the mold halves to fit together in our first two attempts, we used the negative stock to leave function in Fusion on the core side of the mold to ensure that the halves would fit together. We set it to -0.003” on the top, -0.001” on the curved surface, -0.003” on the ramp/draft. The ramp did not close until we added this setting. Lastly, on the adaptive clearing toolpaths on both the goggle core and cavity we reduced the tool load to 10% from the default value of 40% so we were not overloading the tool (on our second failed mold iteration we broke a tool during an adaptive clearing operation due to a combination of overloading the tool and a  lack of coolant fluid).

D. G-Code

Commented G-code from the toolpaths for the blue body cavity mold.

A. Blue Body

Machine & Mold Set-Up: Setting up the Engel for this part was relatively simple. Aside from molding parameters, there was not much deviation from the standard set-up required and detailed in the materials provided. However, fastening the molds to the parts that actually interface with the injection molding clamps presented a few issues. The problems came exclusively with ejectors pins, which were either too short or a bit too long. The pins that ended up being used were the 5.250” pins. These were a bit too short, so the parts that came out had non-negligible places where plastic filled ejector pin holes. There was also quite a bit of trouble getting the ejector pins to align with the mold itself, but we couldn’t tell if this was an issue with the holes or the ejector pins themselves.

Gate Placement: The gate just ran directly into the cavity side of the mold. A simple eyeball estimation is how the runner from the sprue into the mold itself was decided on, as the path chosen looks very close to the shortest path between the two areas. Since the part is largely symmetric, there were no features to avoid, or cosmetic surfaces to protect by placing the gate in a different location.

Injection Molding Parameters: We iterated on multiple configurations of molding parameters, but began with the parameters left on the machine from the last person to use the machine. All parts had a hold time of 8 seconds, and a cooling time of 10 seconds.

Attempts #1 and #2 at injection molding. Short shot and dishing occurred in both of these parts, due to shot size being too small (1.50in), and ejector pins that were too long (5.375”).

Attempt #3. Increased shot size to 1.75in, and shortened ejector pins. There’s less dishing now, but still short shot in the far side (from the mold) of the part

#4 – #8. Changes are just gradual increases in shot size up to 2.30in, and moving the injection boost pressure up to 1800 psi. There is a weldline that still exists at the far side of the part, but since flashing has occurred, we figured the next change must not have to do with the shot size.

#9. Decrease injection speed profile rate.This allowed the injection speed to stay high for longer, which resulted in flashing and burning.

#10 & # 11. Increased injection boost pressure to 2300 psi, and reset the injection speed profile. No more burn, but weldline still present.

#12 – #15. Increased injection pressure profile from 1299 psi – 1650 psi to 1650 psi – 1800 psi. Ran this configuration four times to allow the machine to “catch-up.” Weldline and flashing still present.

Drawbacks: Obvious drawbacks and defects associated with this first run of blue body parts were the flashing and weldline that were created and left unsolved for the time being. Also, another thing that is not necessarily a “drawback” but a “grain-of-salt” observation, is the fact that we did not have any shoulder bolts with our molds. Obviously, this will be a necessary feature in our final parts, so the parameters detailed here may not hold for the final injection mold.

B. Yellow Face

Machine & Mold Set-Up: We needed to use ejector pins closest to 5.353” for the yellow face mold. We decided to use 5.375” ejector pins along with a 0.02” shim to get the ejector pins as close as possible to flush with the part. We reamed the ejector pin holes and did not have difficulty aligning the ejector pins.

Gate Placement: The runner and gate just ran directly into the cavity side of the mold from the sprue since the yellow face part is mostly symmetric and had no features or surfaces to avoid.

Injection Molding Parameters: For our first part we started with a shot size of 2.20” which corresponds to the volume of plastic being injected into the mold. This shot size turned out to be way too large and we has considerable flash on our first part. We then reduced the shot size to 1” which resulted in a short shot. For both of these first two parts we had the hold time set to 10 seconds and the cooling time set to 20 seconds. For the third part we increased the shot size to 1.2” and reduced the cooling time to 10 seconds because the part is relatively thin. This shot size also resulted in a short shot. For our last attempt we increased the shot size to 1.4” which resulted in flash. Moving forward we now know that the holding time of 10 seconds and cooling time of 10 seconds work well and that the shot size will be between 1.2” and 1.4”.

Drawbacks: With the yellow face, the major drawback was the failure of the part to be ejected from the mold. This may be due to the short depth of the sprue hole on the core side of the mold. There may not be enough depth for the plastic to engage with the threads in that hole, so the plastic continually stuck in the cavity side sprue hole. Another problem we saw was that there was a small undercut created by the misalignment of the cavity sprue hole and the hole on the backing plate that interfaces with the clamp. There was quite a bit of overlap between the diameters of those two holes, creating an undercut between the two parts fastened together, preventing the plastic from releasing from the cavity side of the mold.

C. Goggle

Machine & Mold Set-Up: Setting up the Engel for this part presented an issue with the mold height. After zeroing the clamp position and finishing the setup for molding, I tried to mold the part by closing the front gate door. However, once I did this, the clamp began to close, but stopped short of meeting flush with the cavity side of the mold. This happened twice in a row. The error message was cleared, and then we simply re-zeroed the clamp position. The clamp closed fully on the third try, but it remains unclear what the reason was for the clamp stopping short of flush with the cavity side of the mold. The ejector pins used for this part were also the 5.250” pins, and they were much easier to align than that of the blue mold.

Gate Placement: The gate runs from the sprue into a runner that traverses around the outer circumference of the goggle mold cavity. This allows both straps at the sides of the goggle to fill first and have plastic meet in the middle. This allows the gate marks to be at the ends of the straps near the base of the yoyo half, minimizing adverse aesthetic effects.

Injection Molding Parameters: Unfortunately, due to ejection mishaps, we were only able to realize 2 goggle parts, where we varied shot size from 1.50in to 1.25in. The other parameters used in injection molding this part were very similar to those used in injection molding the blue part. The injection speed and pressure profiles were identical to that of the blue base. The hold time and cooling time, however, increased from 8 seconds and 10 seconds, respectively, to 10 and 12 seconds. This was not by design, but simply due to the last person to use the machine using the settings. These numbers, especially the cooling time, can definitely decrease. This part will use less plastic than the blue piece, so decreasing the cooling time will increase our production rate. Again, major flashing still occurred in the 1.25 in shot size configuration, but the issues with plastic getting stuck in the machine made it extremely time intensive to iterate through the different shot sizes and other parameters.

Drawbacks: The major flashing is the most noticeable defect in the goggle part that must be addressed in future iterative processes with the injection molding parameters. However, one of the major features hindering our progress was the failure of the sprue plastic to eject with the rest of the part. When the molds are both clear, the part fills and ejects perfectly fine, but the plastic in the mold cavity sprue hole stays behind. As a result, any molding you try to do immediately after this fails due to plastic not being able to fill the mold because of solid plastic stuck in the sprue hole. Initial hypotheses suggest that it may either be undercutting between the mold and the mold backing part like in the yellow face part. Alternatively, it can be plastic not fully engaging with threads in the core side of the mold, or the sprue ejector pin being too long for the core sprue hole. There was a lot of aluminum cleared from the core side of the mold, so maybe there isn’t enough depth in the hole before the ejector pin fills it.

First Machined Parts

Blue Base

We started machining our blue base mold last week. As expected, there were minimal issues with machining this part, but we did learn a very important lesson about paying attention to the maximum step-down you can impose on a tool path before the tool breaks.

Gray Goggle

The gray goggle core was relatively easy to machine as well. The distance from the top of the part to the lowest point the tool had to reach was relatively large. However, because of the large outer radii of the curved goggle core surfaces, we could afford to use a larger tool that was more resistant to deflection and eventual breaking.

The goggle cavity will be a little more challenging. There are very small radii deep into the mold that will have to be machined with longer but thinner tools. This will raise some concerns for tool crashing and deflection. Some of the issues with crashing have been resolved, but there may be tool deflection that affects the cavity finish. We’d want to avoid this, as the finish issues may translate onto the front of the goggle, which is not ideal.

Thermoformed Dies

We also 3D printed the dies we will be using for thermoforming. The glass dome die (pictured left) was very simple to make, and we shouldn’t have too many problems or defects with these parts. The mouth and hair die (pictured right) will be a little more challenging to work with, and it’s far too early to deem it a successful die. It’s purpose is to fit in the holes left on the yellow face, so we must finish that mold and produce some yellow faces in order to get some feedback on this die’s usefulness.

Next Steps

• Work out machining kinks in gray goggle cavity in CAM, and have the cavity machined by lab’s end (simulated as approximately 1 hour of machining time)
• Finish CAM for yellow face mold, and begin machining
• Begin thermoforming glass dome parts

here we go

Since the last lab, we finalized our yo-yo design and spent some time in Fusion creating the molds for the different injection molded parts we have.

Final Yo-yo Design

Final design changes:

• Continuous snapping surface on the blue base
• Removal of pegs used for secure alignment from goggle to yellow face
• Rounded edges at the interface at the goggle strap and the recessed area of the yellow face
• Addition of black thermoformed piece to fit underneath the yellow face: This was done to remove the extrusions of the hair and the mouth to prevent the yo-yo from causing discomfort in use, but also for aesthetic purposes

Blue Base

The blue base mold was fairly straight-forward to create. The mold was scaled to 1.5% greater than the designed mold dimensions, as per our shrinkage compensation plan. The symmetry of the mold does not present unusual*** challenges (*** = unusual meaning outside of what we’ve already been warned about) for actually injection molding the piece. The more common challenges of getting a uniform part without defects will be what we focus on for this piece.

Goggle

The goggle is also relatively symmetric, and a pretty small piece. Because of its size, we find it should not present unusual*** problems with injection molding either. However, to ensure symmetry, we will need to run the plastic from the sprue hole to the center of the goggle perimeter. We are slightly wary of the distance the plastic must travel to first reach the mold, and then to fill the extremities of the strap uniformly without cooling prematurely.

Yellow Face

oh boy

The yellow face mold is definitely our most challenging mold. With the addition of the black thermoformed piece, we now have complete holes in the part. This creates discontinuities in the mold, and are obstacles for plastic to move around. This creates smaller flow channels in the mold, and may give us problems in getting a uniform piece. We’re still sort of trying to figure out where to put the gate on this mold. We want to avoid the two areas with those feature discontinuities, and we also want to avoid putting it in the recessed area, which is of slightly lower thickness. Preliminary thought directs us to the bottom left or right corner of the face, between the “mouth” and the “cheek”, but we’re still having a little trouble trying to figure out how to navigate filling the thinner recessed section followed by the thicker uniform face area.

I. Final Design

Final Minion Yo-yo Design:

 Figure 1: Side view of full yoyo

Figure 2: Perspective view of full yoyo

Figure 3: Cross-sectional view of yoyo.

Figure 4: Cross-sectional view of yoyo. This view is taken perpendicular to figure 3.

Figure 5: Full yoyo cross-sectional view. Note that the shoulder bolt is longer in picture than the bolt that will be used in the yoyos. The shoulder bolt will be cut to length.

Figure 6: Perspective view of yoyo half

Figure 7: Exploded view

II. Assembly Plan  

We plan to start our fabrication process by machining the goggle strap mold and the yellow body mold as these two parts have a more complicated interface (snap fit and two-pin-press-fit) than the interface between the yellow body and blue body. We will make the goggle strap mold first as that allows us to measure the actual shrinkage of the pegs (and compare it to our estimated values) before machining the corresponding press-fit hole features into the yellow body mold. After we successfully interface the goggle strap and yellow body we will machine the blue body mold, fabricate the thermoforming dies for the goggle glasses and white sclera, and laser cut the pupils from black acrylic. We will use the 1.074” thermoforming punch to cut out the goggle glass part and white sclera part from their respective sheets of formed plastic.

Once all parts are fabricated, we will start the assembly process by stacking the eye on top of the yellow body part. We will stack the white sclera, then the pupil, then the thermoformed dome. Then we will capture those pieces by snapping the goggle strap to the upper ledge of the yellow body part. We will first snap the goggle strap to the yellow ledge then we will press fit the pegs on the strap into the matching holes on the yellow body. While the eye and goggle are being assembled we will use the spacer and set screw to attach two blue pieces together, leaving a space of 0.075” between the two blue parts for the string. We will then snap two fully assembled yellow bodies with goggles and eyes to the two blue pieces to complete the yo-yo.

III. Snap Fit Tolerances

Our design has two traditional snap fits and one pin press fit. The yellow body piece snap fits around the lip of the blue body piece. There is a 0.005” radial (0.01” diameter) overlap between the yellow and blue part for this snap fit meaning the outer diameter of the blue lip is 2.35” and the inner diameter of the yellow part is 2.34” so that the yellow will have to snap onto the blue. Additionally the snap fit surfaces are 0.125” high which is the same height as the snap fit surface on the LMP body part. The second snap fit occurs where the gray goggle strap snap fits around the outside of the upper ledge of the yellow body part. There is a 0.002” radial overlap (0.004” diameter) between the goggle strap and the yellow body part. The inner surface of the goggle strap has a diameter of 1.146” and the outside of the yellow ledge has a diameter of 1.15” so that the goggle will snap onto the outside of the yellow ledge. This snap fit is also 0.125” high. Lastly, the goggle strap has two identical pegs on the underside to press fit into holes on the yellow body part in order to securely hold the goggle straps in place. The diameter of the holes on the yellow body part are 4% smaller than the diameter of the pegs on the goggle in order to account for shrinkage of the pins (discussed in Section IV) and also allow the pegs on the goggle to be press-fit into the holes on the yellow body.

IV. Shrinkage Compensation Plan

    To account for shrinkage, we found a few parts in the lab classroom that had similar features and sizes to those in our yoyo design.

Yellow Body:

This orange piece found in the shrinkage kits was very close to our intended diameter of 2.5 inches. The mold had a diameter of 2.509 inches, and these part diameters were, on average, 2.4333 inches in diameter on the outside edge. This translates to a little over 3% shrinkage. Our important dimensions (i.e. those used for snap-fitting and to lay the gray goggle strap piece in) are affected by this radial change in diameter. Therefore, our initial molds will be approximately 3% bigger to ensure our snap fits will still line up.

Blue Base:

The blue base to our yoyo is another important piece in the functionality of our yoyo. This piece is also intended to have a diameter of 2.5 inches. The parts measured had an average outer diameter of 2.192 inches, which is approximately 1.5% smaller than the mold diameter of 2.227 inches. To ensure that this piece’s snap features line up with the yellow body, we’re going to have the mold diameter of our blue piece be around 2.53 inches.

Goggle + Strap (snap feature):

    These semi-flower pot-esque parts were of similar outer diameter as we expect our goggle diameter to be. The goggle diameter is currently 1.306 inches, and the parts in the kit had average outer diameter of 1.475 inches, flange included. The mold diameter was 1.497 inches, meaning the shrinkage incurred was around 1.5%. We will scale the mold for this part to be 1.5% larger than the intended size of the part, meaning the mold will be about 1.325 inches in diameter.

Goggle + Strap (pegs):

    The pegs from the goggle strap to go into the holes in the yellow body present an interesting shrinkage challenge. We want them to fit snugly with the holes in order to provide some structural support and cohesiveness with the yellow body away from the central circular features. If the pegs shrink too much, then there is no interference between their outer diameter and the inner hole diameter, and the feature has little actual purpose. The shrinkage between these circular extrusions and the mold ranged from 2% to 4%. We will initially plan for 4% shrinkage, but we plan to adjust this number with a lot of trial and error.

V. Injection Molding DFM

We considered the strengths and limitations of the injection molding process when designing our yo-yo. We made the injection molded pieces a uniform thickness of 0.08” so that the parts will cool evenly without sinks or warpage. We also chose 0.08” because this thickness gives our parts enough strength and stiffness to work properly while also minimizing the cooling time in the mold. Since cooling time is the rate-limiting step in the injection molding process, it is crucial to design the parts as thin as possible while not sacrificing any necessary mechanical properties in order to increase the production rate thereby decreasing the cost of the manufacturing process. Additionally, we put a 5° draft angle on the surfaces of our parts that will tend to hug the core side of the mold after cooling. This draft angle will help with part ejection and will ensure our parts don’t get stuck in the mold. We also avoided undercuts in our part designs so that they will come out of the mold. Lastly, we chose to extrude the decorative hair and mouth features of our minion out of the face of the yellow body part so that the molds for this part will be easier to make. The features will formed by making small cuts in the aluminum mold rather than having to make raised skeleton features which would’ve required more material removal and would’ve taken longer to fabricate.

VI. Yo-yo Performance Estimation

Center of Mass:

The center of mass of the yoyo from Fusion 360 is in the center of the yoyo’s horizontal axes, and about ⅓ of the z-direction height of the entire yoyo. This is probably not the exact center of mass of the yoyo as the CADed components are not of the correct density, and the mass will change as a result. However, because the thickness is the same throughout and the sides are symmetrical, we can expect the center of mass to be in the axial center. Once the two halves of the yoyo are put together, the center of mass should balance in the space between them, directly in line with the string.

Yoyo Weight:

    All parts together, including the screw and nuts,  the yoyo weighs 66.59 grams. To calculate this we measured the volume of the individual components in Fusion and multiplied it by the density of Polypropylene of 0.91 g/cm^3 (found on the RTP Company spec sheet for Polypropylene). The mass falls within the suggested range of 60-70 grams for an ideal yoyo weight.