HSM RESEARCH - ON THE EDGE OF TECHNOLOGY
The whole industry seems to be discussing this topic. Here’s what Modern Machine Shop
has to say about "HSM Research - On the Edge of Technology".
Engineering Research Center for Net Shape Manufacturing
The Ohio State University, USA
By T. Altan, P. Fallböhmer
The work described here is part of the current research related to die and mold manufacturing at the Engineering Research Center for Net Shape Manufacturing (ERC/NSM). The information flow and the processing steps involved in die and mold making are presented. Areas in need of improvement are identified and technologies are presented that have the potential to tremendously increase the productivity of a die or mold shop. Among these technologies are computer animation, process modeling with FEA, high performance machining and technology-based CAM.
Modern communication and transportation technology has brought the economies in Asia, Europe and America closer together. A customer or vendor can be contacted within minutes, no matter where he or she is located. Electronic data can be sent through the internet, parts can be shipped around the globe in 48 hours. Therefore, it is no longer sufficient to be prepared for competition in the domestic market. In order to survive, the attention of American die and mold companies has to be focused on the global market. Here, especially Asian countries with their inexpensive labor force play an important role. If a high productivity level is to be maintained in high wage countries such as the U.S., personnel expenses have to be compensated by highly educated and motivated people and utilization of modern technology.
Due to the utilization of advanced technology and a moderate salary level, the U.S. is still the most competitive country in the world, Figure 1. In order to keep that position, American industry has to build alliances with universities to educate employees and implement modern technology.
This is especially difficult in the die and mold business, since tooling shops are small and funds for R&D activities are rather limited. Nevertheless, the die and mold industry has always been regarded as one of the key industries with a need for innovative technology in order to stay competitive. The Engineering Research Center for Net Shape Manufacturing (ERC/NSM) would like to assist the American die and mold companies in facing the challenges of the future. This paper presents work done in technological areas that offer great potential for productivity gains in the die and mold business.
2. Situation In the U.S. Die and Mold Manufacturing Industry
The global market for dies, molds and precision parts is estimated to be $65 billion in sales, with $20 billion U.S. market share. When it comes to increasing global competition, the die and mold business is no exception [Destefani, 1993].
In addition, die and mold making is a dying trade. The average diemaker in the U.S is 56 years old. Soon, the knowledge will retire with them. Young people get more and more reluctant to learn this trade. As a consequence, many tasks on the shop floor have to be automated and traditional skills will be shifted to the engineering departments.
Basics of Die/Mold Manufacturing
Dies and molds are composed of functional and support components. In injection molding and die casting the functional components are called cavity and core inserts. In forging they are called die cavities, and in stamping they are usually called punch and die. Cavity and core inserts are usually machined out of solid blocks of die steel. However, large stamping dies and punches are often cast to near-final geometry with a machining allowance added. In some cases forging dies and injection molds are also manufactured by cold and hot hobbing. Support components are usually standard parts and assure the overall functionality of the tooling assembly in such areas as alignment, part ejection, and heating or cooling. By using standard die and mold components, the time necessary for manufacturing a die is reduced, and machining is mainly devoted to producing the core and cavity, or the punch and the die.
The information flow and processing steps used in traditional die/mold manufacturing may be divided into die/mold design (including geometry transfer and modification), tool path generation, rough machining (of die block and/or EDM electrode), finish machining (including semi-finishing where necessary), manual finishing or benching (including manual and automated polishing), and tryout. In cases where the die/mold shop is a tier one supplier, it might be required to deliver also (a) the part design for a specified functionality and location in an assembly and (b) the finished and inspected parts. This paper presents technologies with the potential to tremendously increase the capabilities and profitability of a die or mold operation. To identify areas of importance, Figure 2 gives an overview of the steps involved in making dies or molds. Some key technologies will be discussed in the following chapters.
3. Key Technologies In Die and Mold Manufacturing
3.1 Communication between Die/Mold Maker and the CustomerRecently the trend towards delivery of subassemblies is becoming more apparent in the automotive industry. Consequently, another challenge to the die and mold business is the trend by OEM’s to request complete subassemblies from their customers or tier one suppliers. Usually the tooling shops have less than 60 employees and their small size makes it impossible to handle the tasks and responsibility that come along with a tier one supplier job. Without proper action, tooling shops will find themselves as tier two or even tier three suppliers with shrinking profit margins. Cooperation will be the key to survival. With further decreasing product cycle times and introduction of concurrent engineering, communication will become the most important aspect in a cooperation between different companies, no matter whether they are supplier and customer or partners in a project.
Therefore, one of the challenges of die/mold shops is to find ways to better communicate with their business partners. Animation software that uses solid CAD geometry as input can deliver the design ideas for complex dies and molds with multiple slides in a much better way than drawings can.
3.2 Process Modeling
In manufacturing discrete parts by using dies and molds, the part design must be compatible with the process in order to assure the production of high quality parts at low cost and with short lead times. Thus, part, process and die design are best considered simultaneously. It is well known that the design activity represents only a small portion, 5 to 15 percent, of the total production costs of a part. However, decisions made at the design stage have a profound effect upon manufacturing and life cycle costs of a product.
Approximately 70-80% of the production costs of a die are already determined during the design stage. [Waltl et al, 1997] Process modeling as part of Computer Aided Engineering, helps to (i) finalize part design, (ii) establish the process conditions and sequences, where applicable, (iii) design the die/mold components, and (iv) minimize the effort for tryout.
Process modeling is being used increasingly in automotive industry to eliminate the need for soft tools and shorten die development times.
3.3 High Performance Machining - Roughing
The high speed milling technology should rather be referred to as ’high performance milling’, a whole system of different technologies that have to be considered in order to be successful. For example, high performance milling already starts in the CAD/CAM system when generating the cutter paths. Accuracy requirements, cutting strategy and interpolation type (linear, circular, NURBS) determine the amount of data the NC controller will have to process later. The high performance milling system will only be as effective as its weakest link.
High speed in terms of feed rate and spindle speed is not always what is really needed. In roughing, for example, the objective of high material removal rates might be better achieved with deeper and wider cuts at slower cutting speeds: The cutting temperature determines the tool wear to a great extent, in high speed milling even more than in conventional milling. Cutting speed is the main factor in heat generation in cutting, followed by chip thickness and width of cut (WOC). Depth of cut (DOC) has the smallest influence because the removal work is distributed to a larger cutting edge area. If DOC is decreased by 50% and material removal rate (MRR) is supposed to be kept constant, the feed rate has to be doubled. If the chip thickness is supposed to stay constant, the spindle speed has to be doubled as well. Consequently, the removal work is concentrated on a smaller portion of the cutting edge. At the same time, this small portion of cutting edge experiences much higher cutting speeds with increased thermal loads. In any case, cutting tools have to withstand high thermal and mechanical loads in roughing applications. Figure 3 shows an extract of results obtained in a project that investigates the potential of high speed milling for manufacturing die casting dies. The H13 with a hardness of 46HRC was machined utilizing fairly severe cutting parameters. The figure shows the tremendous influence of insert design on tool life. Once the material to be cut exceeds a hardness level of 45HRC, chip breakers and other design features that weaken the cutting edge, result in shorter tool life. The reason being that cutting temperatures are considerably higher than in soft materials and chemical wear destroys the cutting edge fairly quickly.
Whenever possible it is desirable to enter the workpiece from the top. The preferred method is to use a helical motion such as that shown in Figure 4. The helical motion should maintain a constant diameter and downward velocity. In order to not have any material left on the top, the diameter of the helical motion should be sufficiently less than two times the diameter of the tool. It is very important to remember that the plunging capability of some tools is limited. The cutter shown has a limit of 16 degrees for ramping motions.
When a cutter approaches a corner the chip thickness as well as the engagement angle increase dramatically, causing a thermal and mechanical shock in the tool, Figure 5. This can be significantly reduced by placing a small arc in the tool path. This condition improves with an increasing arc angle, but with the aftereffect of an increase of material left in the corner. The corner material can be removed using a subsequent profile cut with a smaller tool.
3.4 High Performance Machining - Finishing
The main purpose of the high speed milling technology is to diminish the effort for manual polishing and, at the same time, get the finishing job done as quickly as possible. Improved surface finishes are achieved through an increased number of finishing paths. The step over distance or pick feed in combination with the tool radius determines the theoretical surface roughness. Since the maximum cutter radius is limited by the part geometry, especially fillet radii, the only way to minimize the theoretical surface roughness is to minimize the stepover distance. If better surface finish is required and the stepover distance is decreased by 50%, the number of cutter paths automatically increases by 100%, which means it takes twice as long to finish the part. To compensate increasing time effort, higher feed rates have to be applied. Higher feed rates require higher spindle speeds to assure a constant chip thickness, which automatically results in higher surface cutting speeds. Higher temperatures and accelerated tool wear are the unavoidable consequence. New materials and coatings have to be developed to withstand more severe cutting conditions.
A survey conducted in the die and mold manufacturing industry revealed that, as first priority, 75% of the companies would like to see longer tool life. When finishing a large die or mold, it should be avoided to replace a worn tool in the middle of a cut because it will leave a mark on the surface. Usually it is desirable to take off the 0.010"-0.020" finishing stock in one operation with one single cutting insert. Therefore, in some cases a tool has to last several hours to do the job.
On the other hand, it is absolutely imperative to consider the overall economics when evaluating tooling costs. Tooling expenses represent only a very small portion of the overall manufacturing costs, but high performance cutters and inserts will result in productivity gains that by far outweigh the investment
Ball end mills, bull nose end mills and flat end mills can be utilized in finishing of sculptured surfaces. Unless a die or mold shop belongs to the 6% of American die/mold companies using 5-axis milling, the cutter geometries of interest are the bull nose and the ball end [Fallböhmer et al, 1995]. Bull nose end mills, also referred to as button cutters, are not as popular in the United States as they are in Europe. This is surprising because this type of geometry offers advantages over the ball end, since there is no area on the cutting edge where the cutting speed is zero. The tip of a ball end mill is moving in a linear motion and the cutting speed is zero. This is the reason why metal surfaces cut with the tip of the ball have a dull appearance.
The cutting speed on a ball end mill changes constantly along the cutting edge, it is zero at the tool tip and reaches its maximum on the nominal diameter of the tool. If a 1" ball end cutter is rotated at 10,000rpm, the cutting speed ranges from 0-2600 ft/min. The chip thickness changes along the cutting edge and, at the same time, with engagement angle. These phenomena are referred to as axial and radial chip thinning.
The finishing operation removes the stock left by roughing or semi-finishing. Since the stock allowance is not uniform, the chip thickness changes constantly along the cutter path. Consequently, a mandatory requirement for high speed finishing operations is a uniform stock allowance.
Depending on the application, the finish machining job might look quite differently. In die casting, the high process temperatures require die materials that can withstand thermally induced cracking and heat checking. The hardness of the material, in most cases H13, is therefore kept at 45-50HRC to achieve maximum toughness and thermal stability.
In injection molding, where process temperatures are lower but production rates much higher than in die casting, mechanical wear is of much greater concern than thermal wear. Thus, hardness numbers can go up to 55HRC. Since most often P20 is used as mold material, case hardening is required to achieve these hardness levels. Roughing and semi-finishing should be done prior to heat treatment and the stock allowance for finishing should be kept at a minimum to maintain material properties even after the thin finishing layer has been removed. Forging dies require not only high mechanical toughness to cope with high stresses and impact loads but also high hardness to keep die wear at a minimum. H13 is a popular material, usually hardened up to 55HRC.
Stamping dies are usually cast to near net shape and subsequently machined to achieve the final dimensions and surface finish. Due to low temperatures but high abrasive wear in stamping processes, the functional surfaces in stamping dies are usually flame hardened to more than 60HRC.
To investigate the issues addressed above, expedments were run in cast iron at a hardness of 200HBN and P20 mold steel at a hardness of 30HRC. Cast iron is the most common material used for stamping dies and P20 represents a major player among materials for mold making.
Figures 8-11 show some results of cutting tool tests run at the ERC/NSM. These test are performed on flat surfaces with single flute cutters. The reason being that tool life tests are very time consuming but necessary to determine a cutter’s ability to withstand particular machining conditions. By running tests on flat surfaces and with single flute cutters, the wear is concentrated on a small area of cutting edge and testing time is reduced considerably.
All experiments were conducted on a Makino A55 Delta horizontal machining center. A flat workpiece was machined in climb milling mode at 0.020" depth of cut and 0.020" pick feed. The tool was tilted at 30° to avoid engagement of the tool tip. Cutting conditions were calculated based on a constant actual chip thickness of 0.0025". For testing purposes, Dapra Corp. provided 1" ball end inserts. Among them were plain carbide inserts as well as carbide inserts with TiN, TiCN, TiAIN or TiAI03N coating. In addition, GE Superabrasives provided brazed BZN-6000 PCBN tips on plain carbide inserts. BZN-6000 is a high percentage CBN content cutting tool material. Only inserts with flat rake faces were used, they had no chip breakers.
Cutting speeds varied from vcl000ft/min to 2600ft/min at the highest point of engagement on the ball end mill. Feed rates varied from f=104in/min to 271in/min. Each condition was only run once. To avoid the influence of tool run-out on wear measurements and to speed up the tests, only tools with a single cutting edge were used. The inserts were considered worn out as soon as the maximum flank wear reached VB=300µm (0.012") for cutters used in cast iron and VB=150µm (0.006") for cutters used in P20.
Figure 6 shows the results of tests run in cast iron at a cutting speed of vc=2000ft/min and a feed rate of f=215in/min. TiAI03N outperformed TiN and TiCN coatings by a considerable margin. At the time when this paper was written, the test with the PCBN insert was not finished. However, more than 80,000 linear inches were machined and tool wear was measured to VB=60µm.
When machining P20 at vc=1800ft/min and f=190in/min, Figure 7, the PCBN insert showed a comparable performance. The test was stopped after 100,000 linear inches, which equals 9 hours of actual cutting time. At this stage, the flank wear was measured to VB=80µm. In addition, a PCBN insert was run at vc=2600ft/min, lasting about 30,000 linear inches (VB=150µm). This means that for approximately the same tool life productivity can be increased by 30% when using PCBN compared to coated carbide.
Figure 8 shows roughness values achieved in cast iron. In this case, the measurements were taken when the cutting edge was still new. Not considering the PCBN insert, TiAI03N offers the best performance in terms of tool life and surface finish. In P20, the PCBN tools also yielded the best surface finish, Figure 9. The roughness measurements were taken after the inserts reached the end of tool life.
In general, it is misleading to rely on roughness values only to evaluate the performance of a cutting material. A worn tool may give a better surface finish than a fresh insert, because fresh inserts cut nicer scallops resulting in higher surface roughness. But, since worn inserts also have an offset cutting edge, they leave stock on the surface that will have to be removed manually. Therefore, photos of the surface appearance are shown on top of the chart.
PCBN offers itself as a cutting tool material with great potential not only for high volume production but also for die and mold making. However, special attention has to be paid to its low toughness. Engagement of the tool tip and sudden changes in chip thickness can decrease tool life considerably. To avoid engagement of the tool tip, PCBN should only be used on machines with at least four axis. A constant chip thickness can be maintained with the help of a software package such as the one described below.
3.5 Technology-Based CAM
With current CAM systems, the generation of tool paths for the milling of sculptured surfaces is mainly based on geometrical considerations. These systems provide little assistance for the selection of appropriate milling strategies and parameters. This means that there is some potential to improve the milling process by applying different types of tool path optimization.
The work related to technology-based CAM focuses on optimization of tool paths for the finish milling operations of sculptured surfaces. With the proposed technique (adaptive finish milling), existing tool paths are modified by adding the appropriate spindle speed and feed rate words to maintain the local cutting conditions (cutting speed and chip thickness) within narrow ranges. Compared to conventional milling techniques, adaptive finish milling results in reductions of total milling time and, under certain conditions, longer tool life. So far, only finish milling operations with ball end mills have been studied.
Based on the mentioned deficiencies, current development of CAM systems is aimed at producing NC programs that not only generate the required part geometry, but also take the details of the milling process into account. This approach leads to one or several of the following benefits:
Reducing milling time
Reducing tool wear
Avoiding cutting edge and/or tool shank breakage
Avoiding chatter Improving part accuracy and/or surface finish
In order to accomplish these benefits, tool paths have to be optimized in terms of milling strategy and/or milling parameters. The use of milling parameters (spindle speeds and feed rates) to optimize tool paths can be implemented during the actual generation phase in the CAM system or by modifying existing tool paths.
There are several commercial systems that target the optimization of tool paths. They modify the CAD/CAM generated NC programs by post-processing each NC block. Using a solid model representation of cutting tool and workpiece intersecton, they break linear interpolations (’GOTO’ words) to take advantage of tool path segments where the tool is cutting air. They also regulate feed rate according to the local tool engagement conditions. In other systems, multiple linear segments are combined into a circular interpolation, which reduces periods of acceleration and deceleration, as well as the number of NC blocks processed by the CNC controller.
The proposed optimization strategy (adaptive finish milling) is to maintain the maximum cutting speed within a narrow range by regulating the spindle speed, depending on the local maximum effective diameter of the cutter. In addition, the maximum chip thickness is also maintained within a narrow range by regulating the feed rate. Previous experiments with cylindrical surfaces have shown reductions of tool wear by applying adaptive finish milling [Gaida et al.; 1995].
In order to apply the proposed optimization strategy, it is necessary to obtain detailed information about the local cutting conditions (i.e., chip thickness and cutting speed along the cutting edge). Through a discrete representation of the workpiece geometry and the cutting edge, a chip thickness distribution is generated for a specific tool location within the NC program. The chip thickness distribution, which covers several points along the cutting edge and several rotation angles, is then used to determine the extreme cutting conditions (maximum chip thickness and maximum cutting speed). Then, the spindle speed and feed rate are adjusted to generate the desired levels of cutting conditions.
A prototype software (OPTIMILL) was developed to apply the concept of adaptive finish milling, Figure 10. This software takes an existing NC program in APT format and generates a modified version of the same NC program, with added ’SPINDL’ and ’FEDRAT’ words to achieve a narrow range of cutting conditions [Bergs et al, 1995].
OPTIMILL performs tool path optimization with three major modules. First, the analysis module provides tool engagement and cutting conditions data, at a specific tool location. Based on these data, the optimization module computes the appropriate spindle speed and feed rate. This module also adds ’SPINDL’ and ’FEDRAT’ words to the original APT file, if necessary. In a final step, the workpiece geometry is updated according to the material removed by the current tool path.
The simulation parameters in the input file include resolution specifications for the workpiece representation (mesh) and cutting edge representation (set of nodes). Information about local cutting conditions for both the conventional and optimized NC programs are provided by output files.
Limited testing of OPTIMILL has shown that, compared to conventional NC programs, reductions in machining time of 20-50% are possible [Bergs et al, 1996].
Compensation of Tool Deflections
Once the cutter engagement conditions are known at every location on the geometry to be machined, cutting forces can be calculated with help of mathematical models. Under consideration of the stiffness of the system cutting tool - tool holder - spindle interface, tool deflection can be estimated even before a single cut was made. The existing NC program can be modified, which means specific x,y,z-coordinates will be changed, to compensate the deflections this system encounters [Tönshoff et al, 1995].
As in the past the die and mold making industry will continue be a very innovative industry in the future. To survive competition in a global market, technological and organizational improvements have to be undertaken within the whole production chain. Modern computer technology will (a) facilitate the transfer of information and files between customers and die and mold makers and (b) speed up the design for manufacturing through application of process modeling. This will also save time and expenses further down the road in the production process, since the number of painful design changes will be kept at a minimum. Furthermore, the high performance machining technology in conjunction with the next generation CAD/CAM software offers the potential for a quantum leap in productivity.
Bergs, T.; Rodriguez, C. A.; Akgerman, N.; Altan, T. (1996), Tool Path Optimization for Finish Milling of Die and Mold Surfaces - Software Development, Transactions of NAMRI/SME, Vol. XXIV, pp. 81-86
Destefani, J.D. (1993). Mold and Die Making in Transition, Tooling and Production, 4/93, pp. 69-71
Fallböhmer, P.; Altan, T.; Tönshoff, H.K.; Nakagawa, T. (1996) Survey of the die and mold manufacturing industry, Journal of Materials Processing Technology 59 (1996), S. 158-168
Gaida, W.; Rodriguez, C. A.; Aftan, T.; Affintas, Y. (1995), Preliminary Experiments for Adaptive Finish Milling of Die and Mold Surfaces with Ball-nose End Mills, T. of NAMRI/SME, Vol. XXIII, pp. 193-198
Steinmetz, G. (1997) Germans Falter in Struggle to Regain Competitive Edge, The Wall Street Journal Thursday, June 12, 1997
Tönshoff, H.K.; Meyerhoff, M.; Schwab, J. (1995) Kompensation der Werkzeugabdrängung beim Mehrachsenfräsen von Hohlform-werkzeugen, VDI-Z Special Werkzeuge 9/95, S. 34-36
Waltl, H.; Schulte, St. (1997) Virtuelle Werkzeug-entwicklung - Perspektiven der CAE-Techniken im Werkzeugbau. Proceedings of Werkzeugbau - Eine Branche mit Zukunft!, Hannover 1997, pp. 89-104
Re-posted with permission. Copyright © 1998 by Gardner Publications.
Click here for more industry news from Modern Machine Shop