Introduction

Nature Architects develops product design algorithms that utilize metamaterials. Our goal is to make these products realistically mass producible in terms of delivery, cost, and quality.

This paper describes how to proceed with production design, using the "Folding Hanger" described in Part 1 as a case study. In this product, we proposed a new structure and function by applying a compliant mechanism. We proceeded with the production design concurrently with the functional design described in Part 1.

In Part 2, we present the basic procedure for designing the proposed functionality to be realized with existing mass production technology, in this case plastic injection molding.

Note: In this report, "production design" refers to the study of mold structure, molding processability, cost, and other factors to enable mass production.

Materials, conditions, and terms

Analysis Tools

• Moldflow Insight 2023.
  In this report, it is called “Moldflow”.

Material

• POM、Duracon M90-44（Polyplatics）
  • Thermal Conductivity \(k\) : 0.24 \(W/mK\)
  • Specific Heat \(c_p\) : 2,000 \(J/kg K\)
  • Density \(\rho\) : 1,300 \(kg/m^3\) （Melt）
  • Mold releasable temperature \(T_e\) : 143 \(^\circ C\)

Molding Condition

• Melt Temperature \(T_i\) : 200 \(℃\)
• Mold Temperature \(T_d\) : 80 \(℃\)
• Flow Rate \(Q\) : 50 \(cm^3/s\)
• Filling Time \(t_f\) : 1\(s\)
• Switching position from speed control to pressure control : Automatic calculation（Moldflow）
• Holding Pressure \(P_h\) : 80% of filling pressure
• Holding Time \(t_h\) : 10s
• Cooling Time \(t_c\) : Automatic calculation (Moldflow)

Injection Molding Machine

• Maximum Injection Pressure \(P_{max}\) : 180 \(MPa\)
• Maximum Clamping Force \(F_{max}\) : 7,000 \(ton\)

Brief review of practicality

Injection molding will be used as a practical mass production method. The first step is to examine the feasibility of the process while keeping cost in mind. This stage is a rough confirmation of the following three items. After this stage, a detailed examination is conducted with a modified design.

1. Can the molten plastic be filled into the mold?
2. Are thicknesses of the product appropriate?
3. Can the product be removed from the mold?

The initial shape and dimensions of the foldable structure described in Part 1 are shown in the figure below.

1. Can the molten plastic be filled into the mold?

   • Is the shape too thin for the overall size of the part, i.e., the typical flow length?

     The minimum thickness is 2.2 mm for a flow length of approximately 400 mm (depending on the gate position), which is not extremely thin. Therefore, it can be judged that it can be filled with molten plastic in the injection molding process. On the other hand, the maximum thickness is 6 mm, which is sufficient for filling, and the thickness can be further reduced.

2. Are thicknesses of the product appropriate?

   • Is the molding process time too long?

   • Can the thickness be reduced?

     It is estimated that the "cooling time" in the injection molding process will be longer due to the thicker 6mm at the hook. It is necessary to consider reducing the thickness.

     From the unsteady heat conduction in a flat plate, the cooling time is expressed by the following equation.（Ref.：Rao,Natti S.: Design Formulas for Plastics Engineers, Hanser, Munich(1991) p.50 ）

     \(t_c = \frac{1}{\alpha} \Bigl(\frac{h}{\pi}\Bigr)^2 \space ln \Bigl[ \frac{4}{\pi} \space \frac{T_d - T_i}{T_d - T_e} \Bigr]\)

     where, \(t_c\) : cooling time, \(h\) : thickness of the plate, \(T_d\) : mold temperature, \(T_i\) : melt temperature, \(T_e\) : ejection temperature, and the thermal diffusivity \(\alpha\) in this equation is defined as

     \(\alpha = \frac{k}{\rho \space c_p}\)

     where, \(k\) : thermal conductivity, \(\rho\) : density, \(c_p\) : specific heat.

     The cooling time is determined from the physical properties and molding conditions described at the beginning of this report. For the hook section with a maximum thickness of \(h\) = 6mm, the cooling time \(t_c\) = 35s is predicted to be the time required for the hook section to be ready for removal (”ejection” in injection molding).

     Assuming that the filling time \(t_f\) = 1s, holding time \(t_h\) = 10s, and mold opening to mold closing time \(t_k\) = 10s, the molding cycle time is the sum of the above and is predicted to be approximately 56s.

     

     Note : Regarding the cycle time prediction.

     Strictly speaking, cooling of the molten high-temperature plastic begins when it contacts the mold wall at the start of filling. Since heat input is more dominant than cooling during the filling process, it is practical to assume that cooling begins during the pressure holding process after filling is complete. The purpose of the pressure holding process is to replenish the molten plastic that is shrinking due to cooling, i.e., the heat inflow continues. Although the pressure holding time \(t_h\)=10s is assumed, this is a machine-controlled setting in the molding machine, and the heat inflow may stop in the middle of the pressure holding time. Therefore, the actual cooling time can be considered to include the pressure holding time.

     However, this formula does not take heat input into account, and the time required for cooling cannot be strictly estimated. In other words, the molding cycle time that can be estimated with the above theoretical formula is in the range of 46 to 56 s, and it should be recognized that there are variations. If half of the pressure holding time is adopted, the cycle time can be estimated to be about 51s. However, we would like to estimate conservatively in the initial study.

     The so-called "dry cycle \(t_k\) from mold opening to mold closing can also be increased by setting equipment and devices, but is estimated conservatively as well.

     The following are the results of the Moldflow calculations, which are more realistic because it calculate heat input and cooling in series. The time required for sufficient cooling to allow mold release can be predicted as follows

     　\(t_f + t_h + t_c\) = 42s

     From this, the molding cycle time can be predicted to be around 52s.

     The figure below shows the temperature distribution (cross-section in the center of the z-direction) during the mold release time. It can be seen that the temperature of the hook section, which has a large thickness, is high, i.e., it takes a lot of time for cooling. Conversely, the cycle time can be shortened by reducing the thickness of this section.

     

     Note: Both the theoretical formula above and the Moldflow calculation assume that mold release is possible when all temperatures in the thickness direction reach \(T_e\) (100% solidification). In reality, however, there are cases where mold release is possible even if, for example, the plastic inside the mold is in a molten state at high temperatures, and it is important to promote mold design that allows mold release without molding defects even if the mold is not 100% solidified. Specifically, if the ejector pins are properly positioned, the mold can be removed without applying excessive force during removal and without deforming the part.

     However, it should be noticed that changing the demolding time will cause differences in the cooling conditions within the part. Especially with crystalline plastics, the degree of crystallinity changes, resulting in a change in the shrinkage rate. Shrinkage changes affect the dimensions and warpage of the molded product, which may result in molding defects that were not anticipated at the time of product design. To eliminate rework, we believe it is important to proceed simultaneously with functional and production design of the product.

   Based on the functions required for this product (see Part 1), a certain degree of rigidity is necessary for straight sections and hook sections. Therefore, instead of simply reducing the thickness to shorten the cycle time, it is necessary to design the product to have, for example, an H-shaped cross-sectional shape. This will shorten the cooling time and at the same time ensure constant rigidity.

3. Can the product be removed from the mold?

   • Are there any shapes that are undercut?

   • Is there a draft angle?

     The plane in which the part (hanger) is placed on the floor is the xy-plane. The part is placed so that the mold is opened in the z direction for removal (mold release). The parting plane (PL: parting line) of this part is the xy-plane, the center of the z-direction (z=0). z-direction is the direction of extraction, and the first requirement is that there be no "undercut" shape in order to release the part. Even if there is an undercut, it is possible to make the mold releasable by providing a slide core in the mold, but the mold will be expensive, so we want to design a shape with as few undercuts as possible.
     From the initial study stage of this part, it has already been designed without undercuts.

     In addition, it is essential to provide an appropriate "draft angle" to prevent molding defects during mold release. Generally, the draft should be 0.5 to 1 degree or more. The initial design does not provide a draft angle, so the design must be changed.

     Additional Information: In injection molding, the molded product must remain on the moving side of the mold (where ejector pins are positioned in this side when it opens). Since this product is symmetrical in the +z and -z directions, if the same mold release resistance is used, specifically if the same draft angle is used, the molded product cannot be reliably remain on the moving side. To avoid this instability, this can be achieved, for example, by making the draft angle on the fixed side larger than that on the moving side.

     However, this would break the symmetry in the z-direction. As a function of this product, it is necessary to check the degree of influence of asymmetry. This report does not examine about this.

Design proposal considering injection molding

The proposed design, which takes into account the requirements described in the previous section, is shown in the figure below.

The hook section is H-shaped, and the straight section is T-shaped to reduce the thickness and ensure the necessary rigidity.

Some cross-sectional dimensions of the proposed design are shown in the figure below.

The draft is set at the top and bottom from the center in the z-direction.The thickness of the T-section ribs (the part protruding horizontally in the figure) is a variable to minimize warp deformation in the injection molding process described below, but the initial value is 1 mm.　Preliminary studies have confirmed that the design intent can be satisfied even if the rib thickness is varied between 1 and 2 mm.

Evaluation of molding processability

Now we have determined a shape that is feasible for injection molding. Next, we proceed to check for molding defects using Moldflow.

In the following, we will review the calculation results, assuming the phenomenon of molding defects.

The figure below shows the mesh used in the calculation (only the surface is shown).The two positions indicated by the cone in the lower left part of the figure are used as gates.
In fact, by placing two gates in the bow section, simultaneous filling of three final filling positions (flow ends) can be achieved.However, the two gates were chosen because this bow section is thin-walled and the filling and holding pressure for the straight section should be sufficient (thereby reducing shrinkage of the straight section).

1) Do unfilled defects (short shots) occur?

Simultaneous filling of the three filling ends has not been achieved. However, there were no unfilled defects, partly because the injection rate was set at a relatively high 50\(cm^3/s\).

The temperature distribution of the molten plastic at the flow front (the leading edge of the flow during filling) is shown below. If the temperature drops significantly during the filling process, it will solidify and become unfilled, but in this case, no temperature drop is observed. On the contrary, the high viscosity of the fluid causes shear heating, resulting in a temperature higher than the inflow temperature of 200°C.

2) Are there any weld lines that reduce strength?

The location of weld lines is shown in the figure below.

Weld lines are expected to occur at both ends of straight sections. Especially on the hole side (left side of the figure), a meeting of flows that bypasses the part forming the hole will occur. Since this is the filling end, suppression of weld line strength reduction due to velocity change (see below) cannot be expected for this area.

As a product function, the force that pulls this hole toward the end does not act on this hole, so it is expected that there will be no problem even if there is strength reduction. However, since strength reduction at the weld line cannot be predicted quantitatively in general, it is necessary to actually make and test the weld line, and if the strength reduction is not negligible, then some design change are necessary.
This report does not go so far as to mention this.

The flows from the left and right bows meet near the base of the hook. This is predicted to be the location where the weld line occurs, but this is not the end of the flow, and the flow to the hook section continues after the meeting. At the collision area, back-flow from right to left in the figure also occurs, and further flow continues, causing polymer entanglement, especially in the inner layer. This is expected to keep the strength of this area from decreasing significantly. For confirmation, changes in flow velocity are shown below.

3) Is the cooling time adequate?

Shows the temperature distribution of the plastic in the central cross-section in the z-direction. The figure shows the temperature distribution after about 11 s from the start of filling, the time when mold release is possible. As a result of reducing the overall thickness from the initial shape (time until mold release: approx. 42 s), the molding cycle time can be significantly shortened to approx. 11 s.

4) Are there any sink marks?

The amount of sink marks is shown in the figure below. Although these sink marks (dimples) are not large, 0.04 mm at the maximum, they may be noticeable.

In addition, if the thickness of the ribs in the T-section is large enough to prevent warp deformation of the straight section, which will be discussed later, there is a possibility that sink marks may also occur in the straight section. This calculation result does not predict the occurrence of sink marks on the straight sections.

Basically, sink marks are not a major problem (appearance defect) for the function of this product. If necessary (if sink marks are a concern), the surface can be treated with a grainy finish to reduce the luster and make sink marks less noticeable.

5) Is warpage excessive?

The warpage in the x, y and z directions are shown below.

In the x-direction deformation, it can be seen that the deformation at the bow section is expressed as a large deformation near the boundary with the straight section. This level of deformation (1.5 mm) is not a problem for the bow section, but excessive bending of the straight section cannot be ignored because of the compressive force acting on the straight section during hanger assembly.
In the next step, we will check the relationship between the rib thickness and the deformation of the straight section to determine the appropriate rib thickness.

From the deformation in the y-direction, we can see the change in dimensions due to molding shrinkage. Especially for straight sections, it is necessary to check as a function of the difference from the design of the dimensions.

Warpage in the z-direction indicates deformation outside the xy-plane. The calculated result is about 0.2 mm, which is not a problem.

Although not only in the z-direction, there is still a possibility that warpage may increase due to non-uniform cooling, depending on the cooling channels that can actually be placed. Warpage can be reduced by appropriate cooling channels. The design of the cooling system is not discussed in this report.

Minimize warpage

The thickness of the ribs in the straight section (default value is 1 mm) is varied from 1.2, 1.4, 1.6, 1.8, and 2.0 mm to check the amount of bending in the straight section. Here, only the bending of the straight section is checked, not the deformation of the whole including the bow section. As shown in the figure, one end of the straight section is pinned (fixed deformation in x, y, and z directions, free rotation), and the other end is free in x direction and rotation, to obtain the displacement in x direction of the center section. Since the downward direction in the figure is positive in the x-direction, the amount of deformation is positive if the bend is convex in the downward direction. Since this measurement method is the same for the two straight sections, if they have the same shape, the amount of deformation for both will be expressed as the opposite of positve and negative.

Check the relationship between rib thickness and deformation of straight sections. To do so, we performed Moldflow calculations with rib thicknesses of \(h_r\) = 1.0, 1.6, and 2.0.
The results are shown below.

Note that the end of the straight section appears to stick into the bow in the large deformation, but this is because this calculation does not take contact into account.

In reality, the deformation does not grow any larger because of the contact with the inner surface of the bow, but it remains as a stress due to the restraint and has no small effect on the function of the product.

Based on the above results, the following graph shows the relationship between the rib thickness \(h_r\) and the deformation (bending) of the straight section.
It shows that the deformation is minimum at \(h_r\)=1.6mm.

Revalidation

As in the previous section, we found that to minimize the deformation of the straight section, the rib thickness of the T-section should be 1.6 mm. We will check the sinkage at this dimension.
We see that the sinkage is larger at \(h_r\)=1.6 mm than at \(h_r\)=1.0mm. However, the amount of sink marks is only about 0.001 mm and can be ignored.

Conclusion

We studied the "folding hanger" with a new structure and functions described in Part 1, aiming to realize it by plastic injection molding, which is an existing mass production method.
The necessary design items were studied using theoretical formulas and simulation tools.

Although the mold design requirements have not yet been examined in this report, we predicted the molding defect phenomenon that occurs with the flow and cooling of molten plastic, and developed a shape design to reduce it.

As a result, we were able to determine a product shape that could be mass-produced.
This report does not show the cost reduction effect of integrating multiple parts of a foldable hanger or compacting it. This will be explained in the next report.