Part Cost Estimation................................................................................................................. 4 Mold Cost Estimation...................................................................................................

The purpose of this study is the establishment of techniques that will enable product designers to quickly estimate the piece price and mold cost of an injection molded component at the concept design stage, before engineering drawings are generated. In using these techniques, the designer is made aware of the comparative costs of alternative design concepts, thus improving the product's cost-effectiveness and increasing the designer's awareness of the injection molding process. The capabilities of injection molding will briefly be compared to the capabilities of other processes with the intent of demonstrating when injection molding, and therefore the techniques derived in this study, · may be applicable. The methodology used to determine the three elements (material, processing, and tooling) of total manufactured cost concentrates heavily on input from molding and moldmaking professionals. This is particularly true in the investigation of tooling costs. The result of this research is a costing procedure that does not assume user knowledge of processing parameters

x Fa = appearance factor (from cost is set by product design [1,2]. Efforts to increase the productivity of processing equipment or labor can therefore only impact the remaining 10 to 30 percent of total cost. As a result, the top management of many organizations is placing a greater emphasis on taking the time to investigate design alternatives at the early stages of design. After investigating a number of design alternatives, the concept that a design team would most likely choose to pursue, would either be that which shows the highest ratio of performance to cost, or alternatively, exhibits the highest performance level while meeting a predetermined target cost. Therefore, the ability to make these design decisions is dependant upon the availability of cost estimates for each alternative during the early development phase.
The central goal of this study is the establishment of a procedure that enables product designers to quickly estimate the piece price and mold cost of an injection molded component at the concept design stage, before detailed engineering drawings have been generated. This procedure assumes no user knowledge of process parameters or machine selection, but requires only designer-specified inputs, such as: part size, description of geometry, and material specified.
To be of practical use, costing procedures for each of the manufacturing processes that could be a part of an evolving design should be made available. While this study is exclusively concerned with the injection molding of thermoplastic components, similar work on machining has already been published [3], and studies of sheetmetal, die casting, forging, and powder metallurgy are expected to be completed in 1988 as part of the URI research program on design for manufacture and assembly. Traditionally, designers only have in-depth knowledge of the few manufacturing processes that they tend to use repeatedly.
This often forces them into design solutions that are simply incremental improvements of existing designs. Use of the library of process reports resulting from the research program should broaden a designer's information base, making their use of alternative processes a greater possibility.
Injection molding was chosen for this study because of its increasing acceptance in areas where it was previously thought to be an unsuitable solution. This broadening of applications is primarily due to improvements in material properties and an increased awareness of the processes' ability to produce finished components of widely varying geometry at low unit cost. Although the unit cost of injection molded components is very low, the fixed tooling costs are conversely very high, requiring manufacturers of low-to-moderate volume products to pay careful attention to the trade-off between unit costs and tooling costs. To do this, the means to estimate the cost of the component and it's associated tooling must be made available at the concept stage, before any design commitments are made.
Because of this, early cost estimating is especially valuable to companies producing goods in low-to-moderate volume, and those in industries, where product designs change rapidly and dramatically.
A search of the technical literature reveals that, with the exception of machined components, very little has been published on the estimation of manufactured component costs [4,5,6). Although numerous volumes are devoted to the general nature of engineering cost estimation, the emphasis is generally on projects such as new plant construction, with coverage of manufactured components often relegated to a single chapter. Even within this context, the information presented may be compared to a blank spreadsheet or accounting form, where cost elements and their interrelationships are defined, but the means to actually estimate these cost elements are not provided. This cost information is generally gained through supplier's quotations once engineering drawings have been generated.
By this point, however, schedule pressure generally vetoes any significant changes that appear to be warranted.
The area of estimating tooling costs in injection molding is one where the literature is essentially nonexistent, as seems to be the case for tooling associated with other manufacturing processes as well. This weakness is not entirely without reason, as injection molds are extremely complicated and require many processing methods and design features to accommodate the wide range of components that may be produced. The hazard of trying to estimate costs in this environment is that the required construction and metal removal processes are not apparent to the designer.
The contents of this report can be broadly divided into The intent of this chapter is two-fold: first, to describe injection molding in enough detail that a reader with little exposure to the process will understand its basic workings and cost drivers, and secondly, to convey some familiarity with the terminology that will be used in subsequent chapters.
Before entering into this discussion, it should be noted that this report covers the injection molding of thermoplastics only. Thermoplastics are polymers (the more accurate term for plastics) that may be reprocessed by remelting without significant degradation of physical properties. This is possible due to a lack of chemical bonding between molecular chains during solidification.
Thermosets, on the other hand, undergo a chemical reaction upon polymerization. Following this reaction, the resulting cross-linked molecular network precludes reprocessing.
Common examples of thermosets are: epoxies, phenolics, and some formulations of polyurethanes and polyesters.
Thermosets may also be injection molded in modified machines, although this is relatively uncommon, compared with the widespread injection molding of thermoplastics.
The injection molding cycle may be broken into three phases: injection, cooling, and ejection/resetting. Figure   1 shows an approximate breakdown of how these elements make up the cycle. Each will be discussed in the sections below, followed by a brief description of mold, and molding machine construction. Of the mold through the sprue, after which it follows a series of channels (runners) that carry it to each cavity.
Entering the cavities through one or more small .Reciprocating screws are not the only way to introduce melt into the mold. Plunger machines, utilizing a simple ram and torpedo-shaped spreader to plasticize and inject, were not long ago the industry standard. They have essentially been re~l~ced by reciprocating screw machines, which have the ability to plasticize more quickly and with better control of temperature and shot size.
restrictions, called gates, the melt rapidly fills the cavity. Gates are always the smallest passageway along the melt's path. This causes the material in them to solidify first, thus preventing back-flow out of the cavity. Parts with a sizable surface area will often require multiple gating, as it is desirable to fill the cavity swiftly, before unwanted solidification takes place.

COOLING
Even after the cavity is full, injection pressure is held on the melt in order to "pack" the cavity. Packing results in an increase in cavity pressure, which is necessary to give the part a good surface finish and prevent depressions ("sinks") from forming as the part contracts during solidification. When the gate has been sealed by frozen material, the screw is retracted so that the injection unit can plasticate the next shot. The pressure profile within the cavity is shown in Fig. 3. Cooling of the melt, which began slowly with its injection into the mold, now takes place more rapidly by conduction as the part and mold surface come into intimate contact. Cooling continues to take place within the mold until the part possesses sufficient rigidity to be ejected from the mold.
Part cooling is aided by the recirculation of coolant through passages in the mold. As was shown in Figure 1, cooling is typically the longest element of the mold cycle, and the one that the decisions of the designer, molder, and moldmaker have the greatest influence upon. Factors influencing cycle time will be discussed in greater detail in subsequent chapters.

EJECTION AND RESETTING
Part ejection from the mold is a more critical operation than would appear at first glance. Unless the part is essentially flat, it will tend to shrink onto the male side of the mold during cooling, and can require several thousand pounds of force to remove it. This ejection force must be applied in such a manner that the part will be ejected without distortion. This is not to imply that flat parts are immune to ejection problems, as their inherent lack of stiffness requires that ejection forces be evenly distributed to prevent warpage. It should be noted that most thermoplastics start to soften with a consequent reduction of elastic modulus at temperatures over 225°F. This always results in a trade-off between the desire to remove the part from the mold quickly to reduce cycle time, and the need to ensure sufficient cooling to prevent damage during ejection. Due to the uniqueness of each part, and the particular ejection and cooling characteristics of each mold, the final compromise is arrived at by trial and error.
Ejection is typically performed when pins, blades, rings, or occasionally an entire stripping plate, slide out from their resting position flush with the mold surface, and free the part from the mold. The shape, density and distribution of these ejection elements are determined by part geometry and mold construction (cooling channels in the mold, and any moving slides must be avoided).
In addition to the time taken for ejection, resetting time includes the time required for mold opening and closing. This time is dependent on the velocity profile of the moving half of the mold, and the distance through which it must travel. The magnitude of the mold stroke is mainly dependent on the depth of the part in the direction of mold opening, while the velocity profile is determined by the size and construction of the machine's clamp unit. When the orientation of part depressions or through penetrations prevent the part from being ejected (as in the case of a hole whose axis is parallel to the mold parting plane) , that part is said to be "die-locked''· In these instances, mechanisms called "slides", or "core pulls" are needed to slide these mold projections out of the way so that the part may be released from the mold.

INJECTION MOLDING MACHINE CONSTRUCTION
The basic components of the injection molding machine are the clamp unit and the injection unit. The capacities of these systems are the major cost drivers of the machine and the determining factors in machine selection. Due to their impact on part cost, the clamp and injection unit will be discussed in the next two sections.

INJECTION UNIT
The basic function of the reciprocating screw injection unit was described in section 1.2. As mentioned, there are alternatives to this design, including plunger and screw designs that separate plastication and injection into separate cylinders, thereby increasing maximum injection rates. The industry standard is, however, the reciprocating screw design. Some of the important specifications that determine the applicability of a machine's delivery system to a given job are explained below.
Maximum injection capacity 2 (oz or cu. in.) Theoretical maximum shot size the unit may inject in a single stroke.
Plastication caoacitv (lb/hr) The rate that GP Polystyrene can be plasticated with the screw running continuously. Useful only in a relative sense, as continuous plastication is unrealistic.
Recovery rate (oz/sec) The weight of GP Polystyrene capable of being discharged per second, as calculated following a Society of the Plastics Industry (SPI) procedure. An attempt to arrive at a more useable figure than plastication capacity.
Maximum injection pressure (psi) Theoretical maximum pressure the screw can exert on the melt, assuming no losses.
Maximum injection rate (cu. in./sec) Measured maximum rate of melt displacement at maximum pressure.

CLAMP UNIT
The machine's clamp unit resists the forces developed by injection pressure on the plastic melt as it enters the cavities and runner system.
If this clamp force were Based on General Purpose Polystyrene (spec. grav. 1.04) at 420°F melt temperature insufficient and permitted the mold halves to separate, even by a few thousandths of an inch, material would extrude between the mold plates and cause the part to "flash".
The magnitude of the clamp force needed in a particular application is a product of the plan area of all parts and runners measured in the mold parting plane, and the average pressure within the cavities. Although the pressure drop between the screw reservoir and the cavity is generally 50 %-66% [7], the very high injection pressures result in separating forces that can require the use of machines with clamp ratings well over 1,000 tons.
Besides preventing unwanted mold opening, the clamp unit must open and close the mold to permit part ejection.
The velocity profile of this motion is dependent on the design of the clamp unit. These designs fall into three categories: toggle, hydraulic, or hydro-mechanical.
The kinematics of a toggle clamp (Fig. 4a)  Hydro-mechanical clamps, as one would expect, combine properties of both previous designs. As shown in Figure 4c, a toggle clamp replaces the jack ram of the hydraulic machine to perform mold movement. Clamping is again carried out by a large diameter, short stroke cylinder. This unit combines the faster setup and more precise clamp control of the pure hydraulic design with cycling speeds approaching that of a toggle machine, albeit at a higher price than either.

2.s.o MOLD DESIGN
This section will cover only the basics of mold construction, leaving the analysis of relationships between component design and cost for Chapter 5. The fundamental elements of any injection mold: the cavities, mold base, runner system and ejection system, will be covered in sections 2.5.1 through sections 2.8, followed by a summary of alternative designs to the standard 2 plate mold.

CAVITIES
The surfaces against which the plastic melt is forced during injection sit in two mold plates. The female side of the impression is generally found in the A plate (Fig. 5) on the stationary half of the mold, and is referred to as the cavity, while the male impression is contained in the moving B plate, and generally called the core. The juncture of the A and B plates is referred to as the mold parting line.
Parts that are symmetrical with respect to the parting line make the classification of cavity and core somewhat arbitrary, though the impression mounted in the A plate is generally judged the cavity.
It should be noted that some flat, simple parts have all their detail in one mold plate, while the other, flat plate, simply defines a planer surface.

PROCESSING METHODS
The processing methods used to create these impressions In general, the properties desired in cavity and core insert materials are: wear resistance, toughness, machineablity, polishability, dimensional stability and hobbability (where required) .

FINISHING OF CAVITIES AND CORES
The cost to bring the surfaces of the cavity/core set up to the required level of finish can be surprisingly high; up to 50% of the total cost of the mold (8]

RUNNER SYSTEMS
In any multi-cavity mold, a series of passages is needed to distribute the plastic melt from the central sprue to each cayity. The most critical function of this runner system is to ensure that each cavity receives an equal volume of material. For this to occur, the runners should be of equal length, or "balanced". Examples of good and poor runner systems are shown in Fig 8. In practice, it is unusual to get molds with many cavities to fill evenly without making slight modifications to the sizes of some gates.
The surface finish and cross-section of the runner system are also important to good operation. The surface finish should be as good as the cavity and core surfaces to minimize pressure drops and prevent sticking on ejection. A circular cross-section is preferred, as it presents the minimum surface area for a given volume. This minimizes runner constriction due to melt solidification, although the need to machine both mating mold plates adds to cost.

EJECTION SYSTEMS
The type of ejection system used to release a part from the mold is dependent upon the part's configuration. With these parts, the higher bearing area and a pushing rather than pulling action are needed during ejection.
Runnerless -Eliminates the ejection, handling, and reprocessing of the sprue and runners by heating the entire runner system so that it never solidifies. These heated nozzles become, in a sense, an extension of the injection unit. Often used in multi-cavity molds for high volume parts whose requirements don't allow molding with reground material. Typical examples are disposable medical products.
These molds are expensive and require more skill and experience of the set up person than with other mold types, but can provide very low-cost processing. The three primary categories of runnerless mold designs are: hot-runner, insulated hot-runner and hot manifold.

MATERIAL COST
Because injection molding produces finished components in a single automatic operation, the material cost of parts produced with this method is generally a greater percentage of total part cost than is usual in competing processes.
This chapter will cover the estimation of these costs, assuming the specific polymer resin has been selected.
Descriptions of polymers and their applications will not be presented here, as this information is readily available from a number of sources. A particularly useful introductory treatment is published each spring in the Material Reference Issue of Machine Design (11).

MATERIAL COST FACTORS
The primary cost drivers determining material cost are as follows: lb. each). The list price per pound for truckload quantities of 12 common thermoplastics are shown in Table 1.
List prices are frequently negotiated by moderate to high volume purchasers. The degree to which a resin may be discounted is difficult to predict, as it is dependent on the volatile forces operating on the plastics marketplace.
A February, 1986 survey of the 12 polymers listed in Table 1 reveals that market prices for truckload quantities 1 of these polymers were 0-24% under the list price. Also included in this table is the specific gravity of each polymer, which enables calculation of a more practical measure of material cost: cost per unit volume.

CALCULATION OF MATERIAL COST
An outline of the elements comprising material cost is shown in Fig 13. If it is assumed that the polymer has Railcar quantities for: polyethylene, polypropylene, and polystyrene already been chosen, that its purchase price is known, and that an estimation of part volume is available, then the The impact of runnerless molding on mold and processing costs will be discussed in those respective chapters. If standard cold runner molding is chosen, and sprues and runners are completely reprocessed, the equation describing material cost remains identical to that for runnerless molding. The labor required to gather sprues and runners and feed them into the granulator is usually carried out at the machine, internal to the machine cycle. As such, the influence of runner system reprocessing on part cost is minimal.
As previously discussed, some applications prohibit the use of regrind. When 100% virgin material is a requirement, then the cost of the material contained in the runner system must be considered part of the component's material cost.
To account for this added cost, an estimate of the volume in the runner system must be obtained.
The relationship between part volume and runner volume illustrated in Fig. 14 ( 2) It is unclear if the intent of the authors was that this relationship was valid for single cavity molds only.
Applicability for multiple cavities could be argued, and will be assumed here, as the runner system volume should increase at roughly the same rate as the number of identical mold cavities. In any case, Eqn. (2) should be viewed as only an approximation, as runner volume is quite dependent on part design. The need for multiple gating is an example of a requirement affecting the accuracy of Eqn. (2), and whose need cannot be predicted by those without extensive experience.
The material cost of parts run in a cold runner mold,and requiring 100% virgin material, can now be calculated as follows: ( 3) Now that relationships needed to determine material cost are in place, the processing cost of injection molded components may now be studied.  iThis report will not consider the secondary decorating or coating operations required on some molded parts. Examples of these include: pad printing, hot stamping, screen printing, metalizing and painting.

FILL TIME
Fill time will be defined in this report as the period of time from the initiation of the forward screw motion in the injection unit, to the point where all cavities have been completely filled and cavity pressure is about to rise dramatically, signalling the onset of packing (see Fig 3).
The approach taken to estimate fill time will be to make its The primary effect that this non-Newtonian flow behavior has on the injection molding of thermoplastics is that, because of its impact on viscosity, shear rate becomes a critical factor in achieving desired fill rates and material properties. In short, the molder has an upper and a lower bound to fill time that he must work within for a particular mold. The lower bound is crossed when the fill rate is too low to fill all cavities in the mold before excessive solidification causes a halt to melt flow. On the other extreme, the maximum possible fill rate for a given mold/machine combination is determined by the power available in the injection unit. In some cases, the maximum fill rate is not utilized due to resulting excessive shear rates. Excessive fill rates during filling significantly decrease impact strength, and introduce molding problems such as flashing and burn marks. Whether it is available power or molding considerations that determine fill rate is dependent on the injection power available relative to the shot size, and the part's geometry. The part feature predominant in controlling fill rate is wall thickness.
If the nozzle end of the injection unit is represented by Figure 17, then from elementary mechanics, the work done during injection equals: (5) where W = work, in-lb Pi = injection pressure, lb/in2 Ss = length of screw stroke, in Ab = injection barrel cross-sectional area, in 2 But power equals work per unit time, and Ab*Ss equals the shot size, q. Substituting these equalities into Eqn. (5) A plot of the derived relationship and the original data points is shown in Figure 18. conditions. To account for this discrepancy, and to allow for less-than-maximum fill rates, 0.30 was found to a good general estimate of the parameter fii in Eqn. 6 Mold filling must be completed before the melt has time to solidify through the part's wall thickness. A method to estimate this cooling time will be introduced in the following section.  [17): 10 with the cycle times of a number of widely varying parts, and with several published cooling curves [19,20,21] seem to indicate that, in practice, cooling time increases at a rate somewhat less than the square of wall thickness. The explanation for this very likely lies in the determination of eject temperature.
2 If the maximum wall thickness is in a very localized area which does not perform a critical function, the part may be ejected before this area is fully cooled, effectively reducing the value of hmax used. This is also the case Where the localized increase has greater contact with the mold than is possible for a simple planer wall.
As wall thickness increases, the temperature differential between the part's surface and centerline also and height 3 will be assumed.
Applying gravitational acceleration to determine freefall time, the time required for part dwell between the opening and closing stroke is: (13) where tmd = time for mold dwell, s Ad = die plate area, in2 If the die plate area of a major manufacturer's [23) largest standard mold base is substituted into Eqn. (13) To calculate resetting time from Eqn. (14), the dry cycle time and maximum clamp stroke of the specific molding machine must be known.
Because it is often difficult to get this information directly, the following substitution will be made. Both dry cycle time and maximum clamp stroke are directly related to the machine's rated clamp force, therefore terms in Eqn. 14 containing these variables will be rearranged and expressed in terms of machine clamp force.
The machine catalogues of three manufacturers [13,14,16] were studied to determine continuous empirical relationships where SS = maximum clamp stroke, in If, for a particular application, the quantity (2*d+4)/Ss is close to or greater than 1.0, machine size may have to be increased to ensure adequate clamp stroke. This will incur slight cost penalties due to higher machine rates and a possible slight increase in cycle time.
In a similar fashion, the shot size required for a particular application should be compared to the shot capacity of the machines available to run the job. As with dry cycle time, the following relationship was derived so that a user need only determine required clamp force to make this comparison.
If Q is approximately equal to, or less than the total required shot size q, a larger machine may be needed. Because of the need to provide a balanced runner system, it is unusual to utilize an odd number of mold cavities. Radial runner systems can be an exception, but these are not common for most part geometries. To account for this, the number of cavities calculated from Eqn. (24) should be rounded to the nearest even integer.

CHOICE OF OPTIMAL NUMBER OF MOLD CAVITIES
There are two other instances where the calculated optimum number of cavities may not be the final desired value. The first is when required production rates would require additional cavities. Another reason for non-optimal cavity usage is the lack of available machines of the desired size. This is particularly common for parts of a large plan area and relatively high production volumes.

MACHINE RATES
To calculate the cost of the molding cycle for a particular part, that part's cycle time must be multiplied by the rate charged for the particular machine the job is run on. Because cycle cost is a simple product of these two variables, the accuracy of each value is equally important in determining the accuracy of the cycle cost estimation.
Analysis of machine cost data [24] shows that the purchase price of an injection molding machine increases in an essentially linear fashion with the machine's rated clamp force.
One would therefore expect that the rate charged for use of these machines would increase in a similar fashion.
A summary of machine rates published by Plastics Technology in October, 1987 [30] was the result of a survey of 143 custom molders, and was intended to give a national picture of machine rates. The results are summarized in Table 3.
These values represent the national average for each range of machine size surveyed. Regional variation was Cost estimation involving any goods or services can be described to some degree as an art; it is after all estimation, not accounting. The goal should be to attempt to quantify the experienced estimator's decision making, and to provide a more concrete and informative data base, so that rules can be developed to predict future occurrences.
If this were done, predictions could be carried out by those who are less experienced, as the cost synthesis has to some degree been quantified.
The intent of the following two chapters is to demonstrate that mold costs can be predicted with a

MOLD BASE COST
In this section the cost of producing a finished mold base, defined as all components other than the cavity and core impressions, will be explored. The methodology used assumes that the mold base will not be fabricated from basic material stock forms, but that a standard mold base will be purchased and subsequently modified. Having made this assumption, mold base costs can be divided into the purchased price of the mold base and the cost of modifications to that standard product.
The important parameters defining the cost of a premanufactured mold base are the area of the die plates, and their thickness. Dewhurst and Kupperrajan (24] found that this cost was essentially independent of the height-to-width ratio of the plates and their combined thickness. To relate Ad and Dd to overall part dimensions, the number of cavities contained in the mold must be known, as well as the clearance between the cavities, and the distance from the cavities to the plate edges. Cavity clearances will vary from mold to mold, depending on various technical considerations, the availability of desired mold base sizes, and the practices of each particular mold designer. The average estimate of several professionals in the field [28,32,33,34) was to allow a minimum of three inches between cavities or to the edges of the plate and a minimum of three inches of stock from the deepest point of the cavity to the back of the plate. These clearances generally increase as the overall dimensions of the part, and therefore the mold base, become greater. Die plate dimensions can now be related to part dimensions through the following approximation: Ad=(l+3+0.012*l*w)*(w+3+0.g12*l*w)*n+(3+0.012*l*w) *(l+w+2*(0.012*l*w))*n· +(3+0.012*l*w) 2 (27) where Ad = die plate area in 2 w = overall part width, perpendicular to mold opening, in 1 overall part length, perpendicular to mold opening, in n = number of mold cavities Dd = d+6 (28) = combined depth of die plates, in where D~ maximum depth of part in direction of mold opening Note that Eqn. (27) is an exact representation of area for a square array of cavities.
The use of auxiliary mechanisms, such as a core pulls or unscrewing mechanisms will necessitate additional clearance to the edge of the plate, and behind the cavity, respectively. For this procedure, a doubling of the clearances mentioned will be assumed when these devices are present.
The modifications required of a standard mold base, as discussed in Section 2.7, are generally quite extensive.
The cost of performing this custom work will vary depending on the type of cooling and ejection systems that are  (29) For ease of mold cost estimating, the cost of core pulls and unscrewing devices is considered an additive cost to the mold base.

MOLD ACTIONS
In designing a part that is to be Discussions with moldmakers [27,28,29,36,39] indicate that the simple pull needed to release a round hole would add the equivalent of from 58 to 85 hours of manufacturing cost to the mold. An average of 70 hours will be assumed for each core pull required.
When pulls are needed to release more complicated features than a round hole, the additional cost of creating the feature will be included in the cost of cavity and core impressions, while the basic cost of the mechanism is assumed to remain the same.
When depressions that do not extend through the wall are required on the part's inner surface, standard core pulls cannot be used because the sliding core cannot be activated from the periphery of the mold. To meet this need, a special action, called a lifter, must be used.
Lifters permit core sections to move away from the part's inner surface in order to clear the undercut. These mechanisms are generally actuated by the same mechanism as the ejection system. Estimates of the cost the manufacture lifters into the mold range from 1.5 to 2.0 times that required for core pulls [28,34], therefore 125 hours will be assumed. additional hours (27,28,29). Additional devices required for multiple cavity molds are generally identical , and will cost less than the initial device for reasons similar to multiple-cavity fabrication.
The same exponential index of .80 will be applied to the number of devices (see Eqn. 18) to calculate the total cost of unscrewing devices.
Multi-cavity unscrewing molds are generally manufactured by mold-making shops specializing in this type of work. Typical moldmaking shops will generally not wish to bid on such a job, or will not be able to produ ce it as cost effectively. Estimates of these types of spe cialized molds gained by the procedure developed in this project should be considered very tenuous.

CAVITY AND CORE FABRICATION
The costs detailed in this section will include only those directly involved in the creation of the cav ity and core impressions. After studying literature on mold construction and speaking to professionals in the industry, the following component attributes were determined the primary cost drivers: costs, or were considered to be inappropriate for this study. Some elements of the Sers system pertaining to the remaining 5 items in the list were used in the methodology presented here. The number of hours that each of the seven cost attributes contributes to cavity and core costs will be calculated as described in the following sections.

GROSS PROJECTED AREA
Projected area, along with the depth of the part, determines the amount of material that must be removed, or "roughed out'' before detailed machining begins. As opposed in 3 /min. This metal removal rate is a typical value for vertical milling operations in pre-hardened steel [9]. Note that Xd is not based on the overall depth of the part, but on the depth of the nominal wall from which all projections and depressions emanate. Adding part depth also increases the cost of cavity and core inserts. Using the metal removal rate given above and a cost of three dollars per pound for P20 steel, the cost associated with part depth can be represented as follows: Ap*(Dw-1) xd = ---------+ l*d*w*0.849 120 (31) where Xd = manufacturing time associated with depth, hrs Dw =depth of part's nominal wall (1 inch min.), in

S.3.3 TOLERANCE
From the molder's perspective, the impact of increased part tolerance on mold cost seems not so much the result of more machining hours required to produce the mold, as it is a contingency factor to allow for final fitting, testing, and re-work. Because moldmakers are generally allowed only 10 % to 40% of the tolerance specified for the finished component, they often work close to the accuracy limit of their equipment. Therefore, when extremely high tolerance parts are specified, the moldmaker becomes constrained by the limits of his machine and effectively must take some of the working tolerance away from the molder.
If it is determined that the mold is out of tolerance to begin with, or could not possibly produce a part to tolerance because there is insufficient allowance for process variability, the mold may have to go through one or more re-work loops until the discrepant features are corrected. The Sors work presents a plot of tolerance value vs. additional cost (in hours) However, since it is not realistic to assign a single tolerance value to an entire part design, six classes of tolerance level were created. As shown in Table 4 Table 4.

FINISH
As described in Section 2.6.3, finishing of the cavity and core impressions is carried out with a series of manual operations. When a transparent or high gloss appearance is required, finishing will be a significant component of mold cost.
Since finishing must be carried out on the entire surface of the cavity and core impressions, finishing cost is obviously related to surface area. But since the time required to remove machining marks is proportionally greater in the blends of intersecting geometries than over open surfaces, finishing time is assumed to be more closely related to the square root of the cavity's surface area.
Because of this, the overall geometric complexity of a component will also greatly impact finishing cost. To account for the effect of part geometry, a parameter quantifying complexity is introduced. This complexity parameter is assigned a value between one and ten for the part's inner and outer surfaces. The procedure for determining the parameter values is described fully in section 5.3.7. By studying estimates of the cost to finish parts of dissimilar surface area and complexity, the following approximate relationship describing finishing cost was obtained: Xf = F *A · 5 *C a s av (32) where xf = Fa = As = cav = manufacturing time associated with finishing, hrs appearance factor from Table 5 area of parts outer surface, in 2 (can be approximated by dividing part volume by the average wall thickness) average of inner and outer surf ace complexity levels (from Fig. 25 or Fig.  26) In cases where a photo-etch texture (see Sec. 2.6.4) is desired, a level 2 finish should be chosen from Table 5.
Moldmaker's estimates [28,29,37) indicate that a good approximation for the cost per cavity of a standard texture is 4 percent of the cost of cavity and core fabrication (from Eqn. 34).

EJECTION SYSTEM
Ejection costs assigned to cavity and core fabrication are those costs required to create the ejector elements themselves, and to cut the penetrations needed so that these elements may pass through the core. All costs for additional machining, assembly and fitting are covered under the mold base cost, Cmb· Sors predicts an effective cost of 2.5 hours per ejection pin for making the pin, and drilling and reaming the hole. He leaves it to the reader to input how many pins are required; a task that can only really be handled by experienced moldmakers.
In studying the ejector pin density of 15 parts with diverse geometry, densities ranging from 0.2 to 6.6 in 2 /pin were found. This high degree of variability is not at all unexpected, as the placement of ejector pins is unique to each part's design.
As such, ejection costs are extremely difficult to predict.
The estimating method that will be used in this system is to assume a density of one pin for each 3 in 2 of projected area; the mean density of the 15 parts studied. Since this estimated cost is based solely on projected area, it was incorporated directly into Eqn. 29. While it is recognized that ejector pins are not the only means of part removal, the technique outlined above should provide a reasonable estimated of ejection costs at the concept design stage.

SHAPE OF PARTING SURFACE
The most common surface defining the parting plane at the juncture of the die plates surrounding the cavity and core is a plane. In addition to being the most common, planar parting surfaces are also the most desirable as they are reliable in operation, and the least expensive to produce. Planar parting surfaces (referred to in this study as "Type 1 11 ) are possible when the edge of the part does not description, an alternative method of quantifying complexity has been devised, and will be described in the following section.

CALCULATION OF COMPLEXITY
A weakness of assigning the cost due to geometric complexity by the method described above is that it does not permit designers to assess the cost impact of fairly minor design changes.
For example, a designer would not be able to determine the more cost-effective of two different methods of retaining a secondary assembly, as it would be difficult to accurately assign relative complexity levels for relatively minor differences.
In an attempt to create a more objective and refined approach to defining complexity, a method of counting surf ace patches was devised as an alternative to the assignment of complexity level as described in the previous section. Using this approach for complexity description will more readily permit cost necessitates that additional surfaces must be created so that the insert may be secured, the presence of part depressions or holes carries with it a higher cost than projections. Surfaces that are not reproduced by standard means are those whose shape can be described as free-form because the surface doesn't follow orthogonal planes, or has changes of curvature in more than one direction. A combination of standard features can also fall into this category when their relative orientation dictates that EDM or similar processes would be required to produce them.
Examples of this are a square projection in the part, or a cylindrical projection with a keyway cut into it. Figure 26 summarizes the complexity calculator that was established In reality, it appears that complexity levels in the range 1 thru 10, as calculated using Fig. 26, describe the entire range of injection molded part complexity.
As a summary example, the complexity level calculation of a hypothetical component is detailed in Figure 27.

SUMMARY OF MOLD COSTS
When the seven cost factors covered in sections 5.  In order to examine how total costs are allotted, all components for which a single cavity mold was quoted were assumed to have a total production volume of 100,000. The total cost to process these 100,000 parts were divided into material, processing, and tooling cost so that the relative magnitude of these costs could be compared. The results of this analysis, shown in Fig. 32, reveal that for this total level of production, total mold, processing, and material costs are approximately equal when using a single cavity mold.

INTRODUCTION
Within this chapter, basic considerations in the selection of thermoplastics will be covered. This discussion is by no means intended to be complete in coverage, as the focus will be on processability rather than a summary of property values. To illustrate the use of early cost estimation, a cost comparison of the production of a simple cover plate, in sheetmetal, by injection molding, and by die casting will be presented. The s i ze of the plate and the required load bearing capacity will be varied to determine if these variables impact the relative costs of these processes. Finally, because early cost estimation is sometimes used to aid in the selection of competing designs which utilize the same process, two sets of cost estimates will be developed for an actual injection molded part obtained from an auto manufacturer.  Fig. 33, where the reward for a incremental property advantage is heightened near the target value, and reduced as the actual value departs significantly from this point. One cannot claim a uniquely correct mathematical description for this relationship, nor, due to the subjective nature of ratings, search for an empirical relationship.

IMPACT OF MATERIAL SELECTION ON PROCESSING COST
When comparing the probable relative costs of a group 2 Although injection pressure is dependent on material, the variation in suggested injection pressures is not great for most engineering polymers (See Table 1.) pi = l.12*Ap0.83 (36) where Pi = available injection power, hp AP = projected area of part, in2 Assuming that 30 percent of the theoretical maximum injection power is actually utilized, and that an injection In order to make the relative impact of material selection on cycle time easier to visualize, Table 8 presents a normalized index of the relative cooling times for the thermoplastics whose properties were listed in Tabl e 1. These indices are calculated assuming three different design objectives: 1.) Design with equal wall thickness, 2.) Design for equal stiffness, and 3.) Design for equal strength.
For the latter two considerations, it was assumed that added strength or stiffness was gained by simply increasing wall thickness. The results of Table 8 are presented graphically in Fig. 34.
In addition to its affects on cycle time, material selection impacts processing costs due to the relative processability of each material. This attribute is difficult to define quantitatively, but may be loosely defined as the sum of a number of factors relating to the ease and accuracy with which the polymer may be processed.

MATERIAL AND PROCESS SELECTION
The ultimate goal of the research of which this report represents a part, is to guide designers in the selection of materials and processes.

DESIGN OBJECTIVES
The component to be studied in this cost comparison is a simple cover plate used to seal a square aperture in some kind of enclosure. Figure 35 depicts this plate in the two configurations studied here: flat and ribbed. The following design and production requirements were assumed: 1. Cover must be removable, though not regularly.
3. Sealing of anything other than dust and light is not required.

4.
Production volume is fairly low. Costs will be analyzed for total production of from 4,000 to 28,000 covers.
5. Covers will be used over a 2 year period, with production orders placed twice per year.
In order to present a greater range of comparison, two separate design objectives were chosen for study. The first was to assume a maximum allowable deflection for a series of In order to analyze comparable designs, it was assumed that the method of attachment for all designs was by four screws.
Because of this, an estimation of assembly costs was not required. In practice, many injection molded components of this type would be designed with integral snap elements that would eliminate the need for screw fastening.
In the next section, the cost of providing these features in the mold will be compared to the savings in assembly costs and fastening hardware.

CALCULATION OF COST ESTIMATES
The following combination of materials and processes were analyzed as solutions to the two proposed design objectives.  [43).
Because this comparison is being made for relatively low production volumes, it was assumed that the sheetmetal parts would be punched on an N.C. turret press without the need to purchase special tooling. The amount of scrap produced in the web between the parts becomes greater with increasing plate size because it is more difficult to lay out the pattern efficiently on the sheet. Although there is usually a salvage value of approximately 10 percent of purchase price, it is not substantial enough to alter the final result of process selection and for this reason will not be included in this comparison. Times for stamping and finishing were estimated, after some modification to fit the proposed situation, through standards published by Ostwald [24). Cycle times for die casting were estimated based on shot weight [42).
The mold cost of a die cast component is somewhat higher than an injection mold would be for the same component, although their construction is nearly identical.
Part of this difference can be explained by the more costly mold materials required to resist the extreme temperature cycles present in the die casting process. This aspect of thermal shock also increases the maintenance costs of diecasting tools. On the other hand, the surface of cavity impressions used in die-casting do not have to be finished to the high degree that is required in injection molds.
Flash is always present at the parting line of die cast components due to the extremely low viscosity of molten metal, requiring a secondary piece of tooling, called a trim die, to remove this flash. For this example, an estimate of the additional cost of the die cast tooling and trim die over that of the comparable injection mold is 20% [43).
Nickel plating, common for die cast components was assumed the finishing method. As estimated using [24), this cost should be approximately equal to that of painting sheetmetal plates of the same plan area.

ANALYSIS OF RESULTS
The total estimated costs of producing cover plates, designed for variable size and for variable load are summarized in Tables lOa-lOd and lla-lld. Figure 36 presents plate cost vs production volume for the 2 inch and 12 inch plates, the total production volumes ranging from 4,000 to 28,000 units. The divergence in costs in going from the 2 inch to the 12 inch plate is explained by the increasing influence of material cost. Moreover, the breakeven production volume required to justify injection molding increases when the plan area of the part increases, as machine rates are very sensitive to this variable. In Fig.   37, costs are displayed for the entire range of plate sizes at a constant production volume of 10,000 pieces. This figure clearly shows the high material cost of aluminum sheetmetal parts, as the relatively high cost per cubic inch is magnified by higher scrap costs, the much coarser graduations in material thickness and the inability to reduce part volume by ribbing when designing in sheetmetal.
For the other materials, note that the relative costs are unchanged as production volume is varied. As can be expected, this is also the case when designing for variable loading (see Fig. 38).
Wall thickness of the zinc parts range from 0.040 to 0.090, which essentially covers the entire range of recommended wall thickness for zinc die cast parts. This fact, coupled with the results of Fig. 38 seems to lead one to conclude that die casting is not competitive when considering a factor for which it would seem better suited to than injection molding; namely stiffness. However, referring back to the beginning of this chapter, it must be noted that if consideration of constant long-term loading and extreme use temperature were required, then this conclusion would almost certainly change.
In examining Figs. 36 through 38, the reader may be surprised that the polypropylene designs are consistently more cost effective than those molded in glass-filled polyester. Even though it is talc-filled, polypropylene is an inexpensive polymer not generally considered a prime material choice where stiffness is the major design consideration. While this study projects that injection molded polypropylene is the most cost effective combination of material and process for total production volumes of greater than approximately 14,000 units, the impact of the very long cycle time associated with injection molded parts of a large wall thickness is not fully accounted for. For the relatively low 4,000-28,000 total output assumed in this study, a one cavity mold is underutilized even if operating at very long cycle times. But if required production rates are raised to a level high enough that multiple cavities are more economical, the polypropylene parts will require more than double the number of cavities than for parts made in polyester due to the much greater cycle time required. In this case the penalty in additional tooling cost would be substantial.

ASSEMBLY COSTS
In order to make a direct comparison of equivalent designs, the method of attachment was universally assumed to be by threaded fasteners. In many designs however, snap elements are utilized for the attachment of injection molded parts. A characteristic common to all snap elements is an undercut that provides the retaining capability. When the axis of this undercut is other than parallel to the direction of mold opening (which is generally the case) , ejection of the part from the mold is inhibited or prevented. Some thin-walled parts with undercuts, such as snap-on lids, can be stripped from the mold due to their ability to flex. When sufficient flexure is possible, the part protrusions will pass over the undercuts in the mold.
Since the need for expensive core pulls are eliminated when undercuts can be stripped from the mold, this type of integral fastener is the most cost-effective method of securing components. Nevertheless, stripping undercuts is not generally possible when the feature is prominent because flexure is limited by allowable strain. The very low levels of allowable strain characteristic of glass reinforced polymers make them poor candidates for use with stripped parts. Allowable short term strain for this family of materials is about 1.5%, as compared to approximately 4.5% for non-reinforced grades [46].  Table   12 summarizes the cost of installing the six inch plate assuming the following installation systems: four self tapping screws; four sets of nuts, bolts and washers; four machine screws and Pemsert hardware; and by using four integral snap elements created by two separate sliding cores. Assembly costs were estimated using Boothroyd-Dewhurst Design for Assembly [44] analysis, assuming a burdened labor rate of 30 $/hr. In Fig. 39, the assembly cost of each system is plotted for a range of production volume, amortizing the estimated $4,550 cost of slides into the snap-fit assembly cost. Examination of this confirms what is readily apparent in current designs; that snap elements are an extremely cost effective method of joining components. What seems not to be so apparent to many manufacturers is that low-volume production does not preclude taking advantage of the benefits of injection molding when assembly costs are considered.

EFFECT OF PART ATTRIBUTES ON COST
A valuable benefit of making this type of procedure available to product designers is that it gives them guidance in a quantitative rather than axiomatic fashion.
To illustrate how design variations may be judged quantitatively, Fig. 40 illustrates the impact on mold cost of a 20 percent increase in the average values of each part attribute in Table 6.
A more specific example of evaluating design alternatives involves a heater system component (Fig. 41) obtained from an automotive manufacturer. In examining the part, it was evident that the thickened pads greatly increase the cycle time over what would be possible had the part been designed with a constant 2mm wall thickness. As an exercise in comparing alternative designs, this part was redesigned so that the mounting pads were cored out, leaving a constant 2mm wall (Fig. 42). Although it was certain that the cycle time, and therefore piece part cost would drop significantly, it seemed that the increased cavity detail needed to create the ribbing would just as surely result in the need to maintain some minimum production volume for the change to be cost-effective. The missing element in this train of thought is that, if the cycle time reduction is great enough, fewer cavities will be required to maintain the same production rate, making it possible to reduce both piece part cost and mold cost. That situation turned out to be the case for this redesign. The estimated 63 percent decrease in cycle time permitted a reduction in the number of cavities required from six to two. Although the cost of a single cavity/core increased due to greater cavity complexity, the need for only two cavities permitted an estimated 28 percent decrease in total mold cost. The net result of this proposed redesign is an estimated 21 percent decrease in part cost, as shown in Table 13.

APPLICATION OF RESEARCH
The methodology outlined in this report has been developed for use by designers as a tool in optimizing material and process selection at the concept design phase.
Early cost estimation techniques are most effective when Many manufacturers felt comfortable with threaded fasteners and were apprehensive of designing with snap features, feeling that they carried a much higher risk due to creep, yield, or fracture. As some manufacturers decided to take this risk, it became apparent that, when designed and used correctly, snap features were in fact much more reliable than threaded fasteners. Those organizations that were among the first to use snap features not only got a head start on bringing more cost effective goods to market earlier, but developed a new expertise first-hand and gained confidence in taking the road of innovative design.

FUTURE WORK
Areas of future investigation can be divided into those pertaining specifically to early cost estimation of injection molded components and those that apply to early cost estimation in general. Areas of this report on injection molding that could be strengthened or expanded deal mainly with estimating the mold cost due to part                                11 2" 4 11 6" 9" 12 11 Table 6. For tolerance, finish, parting surface, and complexicy the added cost was calculated based on increasing the index for thac atribuce by one.