Deliverable 3

Thankfully, shooting two parts in one mold was successful.  We had doubts as the overall surface area of our parts was quite large.

Fro and I spent a couple of hours with the injection molding machine, adjusting parameters like extrusion temperature, rate, cooling time, and the pressure profile.  The end result was a pile of data (pictured above).

We optimized to reduce shrinkage around the critical dimensions, those being the press fits for the bearing and ballast nuts.  The nut press fit was very tolerant of changes in shot temperature and cooling time.  The most extreme values deviated by no more than three thousandths of an inch from one another.
The bearing press fit dimensions were more variable. The OD of the bearings we're using is .315", we aimed for an interference fit of ten thousandths.  Regardless of variations in parameters, the dimensions stayed very consistent.  However, we found that the cavity shrank into the shape of an ellipse.  The major diameter averaged to about 0.311" while the minor averaged to 0.307". 
This made for 0.009" and 0.013" of interference respectively.  The fit was slightly snug, but went easily with the help of an arbor press.

Later, we increased cooling time to 30 seconds in an attempt to further refine dimensional accuracy.  During our trial run with clear plastic, this did not pose any issues.  However, when we added black dye to the plastic, the results were catastrophic.  Bowties wedged themselves in the core and punctured or cracked when the ejector pins were fired.  Although the critical dimensions were preserved, the parts were not.  We observed that this was provoked by long cooling times. We solved the problem by reducing the cooling time from 30 to 20 seconds, and by using copious amounts of mold release spray on the core. 

We also had to tweak the feed stroke to maximize packing while preventing flash.  We did this by trial and error, increasing the value by 0.05 cubic inches from our initial value of 1.6 to our final value of 1.85.  We noticed flash began to appear at around 1.95 cubic inches.

The injection hold pressure profile did not require changing.  We played with the values to see their effect on the part, and found that it had none in the range to which we changed them.  They seemed uncorrelated.

One of the damaged bow ties.

The remainder of the parameters were unchanged.

A full production run, mostly successfully

Process Parameters Sheet:

Injection Hold
Injection Hold Pressure Profile P7-P16
653	600	600	600	600
600	400	376	350	350
Injection Hold Time			Z2 =	8s
Cooling time			Z4 =	20s
Set Screw Feed Stroke			C1 =	1.85 cubic in.
Injection Boost
Injection speed profile: V12-V21
6.3	6.3	6.3	6.3	6.3
6.3	6.3	6.3	6.3	6.3
Injection Boost Pressure			P6 =	1100 psf
Screw Feeding
Screw Feed Delay Time:			Z3 =	20s
Ejector
Ejector Counter			AZ =	2
Ejector Pin Lengths:	4x 5.690 in.	6x 5.570 in.	1x Sprue
Total Shim Thickness:	0.062 in.

Deliverable 2

Description of Mold Design

                The molds for the bowtie parts of our yo-yo were manufactured out of two 6061 (T6) Aluminum blocks (Figure 1). All of the features on the mold were milled on the EZ-TRAK mill. Two identical bowties are molded in a single injection molding run in order to reduce operation time and cost. This was done by creating mold features for two bowtie parts on each mold part. Runners on the cavity mold link the sprue to each of the two sets of parts.

Figure 1. Photographs of machined (a) cavity and (b) core molds for bowtie parts.

                The core mold (Figure 1b) was designed to form the concealed lower ribs that provide structural support for the part. It consists of extrusions that will obstruct the flow of molten plastic during injection molding, and will slide out from underneath the part once it has cooled.
               The cavity mold (Figure 1a) was designed to form the outer surface of the part. It consists of a rounded pocket that will provide the visible upper surface of the part has a smooth, aesthetically pleasing surface finish. It will slide out from above the parts once they have cooled. The parting line of the mold was chosen to lie at the lower plane of the part in order to allow for easy removal of the mold once the part cools. Since the bottom face of the part will be concealed in the yo-yo, any minor defects due to misalignment at the parting line will be concealed.

                The molds include circular holes towards the sides, which ensure that the intended positions and orientations of the core and cavity molds relative to each other and to the injection molding machine are attained. All other features serve to form the parts themselves by directing the flow of molten plastic during injection molding runs.

Quantitative Justification of Dimensions

The bow tie cavity mold was machined to the nominal dimensions.  Since the bow tie is an aesthetic element, shrinkage during injection molding was not considered to be an issue.  The critical dimensions on the core are for the interference fits of the bearing and ballast nuts.

Based on measurements of previous years' parts, we estimate a shrinkage of 2% from the mold dimensions.  The nut has a diameter of .438".  We cut the mating feature in the mold to a diameter of .433"  With an additional 2% of shrinkage, we estimate the interference fit for the nut to be .014"
 
The bearings to be used have an OD of 8mm or .315".  Accounting for shrinkage, we machined the corresponding core mold feature to have an OD of .315".  2% of shrinkage yields an interference of .006"

Description of Manufacturing Process
These molds start from a premade mold blank.  The mold blank is designed with locating holes and a sprue.  The locating holes are used to repeatably fixture the mold to the EZ-TRAK mill bed, and also to the injection molding machine.  A CAD model of the mold is imported to MasterCAM, where toolpaths, depths of cut, and feed rates are specified.  The resulting tested G-code is then taken to the EZ-TRAK, where machining happens.  A human operator monitors the process and changes tools.  After machining, some post processing may be required.  Holes or sharp edges may require deburring.  It is important to avoid deburring or rounding any surfaces that when rounded, might create flash.  If desired, the mold surfaces may be lightly sanded to remove machining marks that may be displayed on the finished injection molded part.

Link to our process plan

Mold Details

The core mold was milled successfully. We even managed not to break the 1/16" end mill when it accidentally cut the full depth of the grooves (all 5/32") in one go. If we have to remachine, we will not be making that mistake again, despite the increase in milling time.
The face of the mold, while appearing patterned, is incredibly smooth, which is important for fitting against the cavity. Any grooves or roughness to the surface would have made flashing more likely. The top of the islands do not need to be finished, as they are not touching the cavity at all. Also, since the sides of the islands remain unseen, they did not have an additional finishing pass applied to them. Since it seems that being slightly rougher will not have an impact on removal from the mold (according to David when I asked him), there is little point in changing that.
If reworking is required, probably decreasing the size of the bearing island (center circles) and increasing the size of the hex nut islands (large trapezoids) to accommodate better press fits will be done.

In spite of its dashingly good looks and polished interior (which was done manually, post-milling to improve surface finish on the injection molded part), the cavity mold was machined to a depth that is 1/16" too shallow.  It would result in a bow-tie with voids where the core unintentionally comes into contact with the cavity.  The operator has made plans to remachine the cavity mold, bringing it to the correct depth.

Deliverable 2-b: Time Table

Component Time Table

Component	Time per Part	Number of Runs	Total Time for parts	Component Total Time
Bow Tie
Bow Tie Cavity Mold	42 min 10 sec	1	42 min 10 sec
Bow Tie Core Mold	35 min 56 sec	1	35 min 56 sec
Bow Tie Injection Mold	0 min 15 sec	105	26 min 15 sec
				104 min 21 sec
Retaining Ring
Ring Cavity Mold	45 sec	1	0 min 45 sec
Ring Core Mold	41 sec	1	0 min 41 sec
Ring Injection Molding	8 sec	210	28 min   0 sec
				29 min 26 sec
Window
Window Thermo-Mold	1 min   2 sec	1	1 min  2 sec
Window Thermo-Forming	0 min 35 sec	210	122 min 30 sec
				123 min 32 sec
Yo-Yo Body
Body Cavity Mold	3 min 43 sec	1	3 min 43 sec
Body Core Mold	6 min 14 sec	1	6 min 14 sec
Body Injection Molding	0 min 20 sec	210	70 min 0 sec
				79 min 57 sec
Extra Set-Up
Preparing Machine per Component	10 min	4	40 min
				40 min
Yo-Yo Assembly
Assembling a Yo-Yo	3 min	100	300 minutes
				300 minutes
Complete Fabrication of Project				11 hours     17 minutes 16 seconds

Part Assumptions:

Bow Tie: We are trying to mold two bow ties at once.  We assume that the surface area of the mold is not too great for the injection molding machine.  If it is an issue, we will modify the mold, blocking one of the channels and reducing the apparent surface area.

Retaining Ring: We are assuming that the constant thickness will cause the mold to cool at the same rate at all parts of the ring. Because of the small thickness, there should be no need to a small draft angle to help the ring be ejected from the mold. Because of the lathe and small amount of mill work, creating this mold will take very little time. We also assume there will be approximately 2% shrinkage with this part, based on measurements of model parts in the lab classroom. Thus, the mold dimensions are 2% larger than our final goal dimensions.

Thermo-form Window: We are assuming that the thickness of the thermoformed part remains roughly constant, so that the upper profile of the part is an offset of the lower profile. We are expecting a variation in thickness of within 10% throughout the part.

Yo-yo body: We have assumed a 2% shrinkage of the body upon cooling, and so we have scaled the molds by 102% to accommodate that.

Injection Mold Assumptions:

We are going to create 210 molds for each part to ensure that all molds fall into our tolerance range and do not have any deformations.

The bow tie, a complex but thinner part, will take about 15 seconds for each body to cool. The bow tie mold can complete two bow ties at a time, therefore waiting 15 seconds gets two bow ties done at once. This is why only 105 runs are required to create 210 bow ties.

The retaining ring is the thinnest part, thus we assume it will only take 8 seconds per part to cool.

 The thermo-formed window is a bit slower than injecting molding because of the heating of the plastic, thus will take 35 seconds.

The yo-yo body is the thickest part, thus it will take the longest to cool. We will assume it takes about 20 seconds for each body to be made.

Because it takes about 10 minutes for the set-up of each molding process (warming up of plastic, loading G-code, etc), an extra 40 minutes must be added onto the fabrication process. We estimate that it will take 4 hours, 7 minutes, and 30 seconds to fabricate all of the plastic parts to make our yo-yo.

Once all of the parts are created, we need to press fit together all of the parts. For each yo-yo, it will take about 3 minutes to assemble one yo-yo. This includes press fitting parts together, screwing in one side of the yo-yo into the other, and checking for errors. By using all six group members, we can create an assembly line to put together yo-yos in about 5 hours.

Conclusions:

The time schedule above dictates how our team will spend our time in lab. Our team must set time aside during the week to come to lab to manufacture parts. It is also important to complete all parts by a particular date to begin the assembly of our entire yo-yo. If any part needs to be re-done, using the table determines how long we need to spend in lab to fix mistakes. As parts are changed, our group will edit the time table to keep an accurate time table of fabrication time.