|
|
|
|
   
|
||||||
|
|
INSIGHT
High-performance machining is a comprehensive approach that takes into consideration existing and potential machine tools, tooling, tool holders, fixtures, part processing, and machining strategies. HPM can best reach machining objectives when a shop uses the best technology available to machine its components, regardless of part, feeds and speeds, or type of shop. Here's an HPM approach to putting new tooling and machining strategies to work in the shop. For best results, all aspects of HPM must be considered. Neglecting any one facet means a shop will not realize its full potential benefits. A five-step plan 1. Make improvement priority one-Moving toward high performance machining must be someone's official job. While an individual should be designated to lead the task, the project must be a team effort. The team should consist of management, manufacturing engineering, and shop floor workers with authority to purchase what is needed to make the desired improvements. 2. Evaluate strengths and weaknesses of current machine tools- Not all machines, even those with the same specifications, perform the same way. Every machine has its strengths and weaknesses. In order to improve, shops must take stock of their current machining environment by evaluating their manufacturing processes and identifying the most-time consuming ones as a starting point for their first efforts. Brake caliper: preliminary part, 16.25" x 8.3" x 3" thick block of aluminum. Screen capture illustrating straight-line cutting recommended for milling applications. Testing A New Tool 3. Research tooling and machining strategies-Machine tool suppliers and their applications team should be contacted for advice on processes and relationships should be developed with tooling suppliers. Knowledgeable tool vendors are an excellent source for recommendations on how to best apply the machine and cutting tools, as are other sources such as machine tool shows, machining seminars, and trade magazines. 4. Compare old methods with the new-Run tests by processing parts on available cutters using the techniques and strategies suggested by previous research. Record the speeds, feeds, and depth of cut that yield optimum metal removal rates and stability. Based on these results, shops can browse catalogs and order some new tooling for additional testing. For example, take a block of scrap material, put it in a vise and make some very simple test cuts. Experiment with various machining strategies, record results, and apply them to the next part processed, all the while striving to improve upon machining time and tool life achieved with the old methods. Shops that do one-of-a-kinds may be skeptical about running the above test on good material because they do not want to take unreasonable risks of scrapping a part. They also probably realize that they cannot afford to stay with the old machining practices either. However, these shops can test single-lot size production runs by repeating similar types of operations on different parts and making incremental changes. One-ofa-kind shops often drill and tap the same size holes in many of their parts and make milling cuts with similar cutting conditions, tooling, and speeds, feeds and depth of cut. In effect, they repeat processes, but not exact parts. These are the processes that these shops need to improve first before applying the new process. 5. Pick best performer and put it into productionAfter testing, shops can determine which combination produces the greatest improvement. It may be that by simply adjusting the depth and/or speeds and feeds of cuts, the desired result can be achieved with existing tooling. Or, shops may find that they must purchase new tooling and reprogram portions of the part program in order to maximize the new machining strategies. Whichever path is chosen, the plan should be put into action on the shop floor as soon as possible. A case in point CAM software enables routines developed for the caliper to be applied to machining a vacuum chamber. A good example of realizing the benefits of HPM comes from a shop machining a large aluminum brake caliper. Beginning with a 16.25"x8.3"x3" block of aluminum, the shop found one cut especially problematic: milling the outside of the part to a depth of 3.0". Because of the size of the inside comer radius, the tool diameter could not exceed 1.25". The customer opted to use a 1.25" solid carbide roughing end mill with a 4.0" flute length that was specifically designed for aluminum. The shop found that when the width of cut was more than half the tool, it would chatter and--on occasion-the tool would even break. The goal was to find a machining strategy that would eliminate the chatter, improve cycle time, and increase tool life. Following the HPM approach, the customer did the necessary evaluation of current tooling and researched new machining strategies. It made sample slotting cuts with available tooling and ran these same tests again with new tooling ordered from catalogues. The new tooling, optimized for speed, feed, and depth of cut, produced a 30 percent increase in productivity. The tests run with the new tooling demonstrated that running this tool at 2,700 sfm with a 0.0145 ipt (8,250 rpm/120 ipm) yielded a solid sounding cut and great tool life. These results are somewhat surprising because while the sfm is not too unusual for aluminum, the almost 0.015 ipt feedrate is very high for a single-flute tool that is hanging 3.5" out of the tool holder, but still within the recommended range for the tool. The shop would have been skeptical had they not conducted the necessary tests and seen the results themselves. Evaluation, testing, and process change were completed in one day. CAM as an ally Computer-assisted machining (CAM) is a tool that shops can use to help in the process of accumulating data for such test cuts. Flexible CAM systems store machining knowledge and preferences in a database that can be accessed quickly for use on any part. The ideal software not only has a strong set of standard machining cycles that can be easily augmented, but it also enables programmers to create customized routines that extend beyond the ordinary tool path. In particular, CAM that includes Visual Basic facilitates this customization by supplying an industry standard macro language. CAM with realistic simulations show the machining in the same manner as the machine really moves, aiding shops in previewing new machining strategies and seeing what impact they have on cycle time. This feature is particularly useful on multi-sided parts machined with rotary tables. When running a difficult part, shops can use a PC out on the shop floor to quickly update the toolpath, simulate the changes in the CAM system, DNC the code to the machine, and start cutting. A good example of how CAM can benefit a shop comes from a customer machining a part for a vacuum chamber. The shop used the same tool and machine process developed for machining of the previously mentioned aluminum brake caliper to rough machine the chamber's three large pockets. The appropriate tooling and machining process had been saved in a CAM system and thus was available for future applications. Different part, different machine, different customer-but a similar process. High-performance machining isn't about cutting comers. It's about putting the best technology to use on the shop floor and capturing that knowledge for future machining jobs. DP Technology, Camarillo, CA, Optimizing Strategies The following tests can be used by all job shops, including those machining "one of a kinds," to improve their machining strategies and make the move to high-performance machining. 1. Start with the mid-range speeds and feeds from the tooling manufacture. 2. Make straight-line, slotting cuts, starting with a shallow depth of cut (like 0.1" deep). 3. Increase depth of cut until chatter occurs (usually at 0.05" or 0.1" increments). 4. At the maximum depth cut without chatter, increase feeds and speeds toward higher end of recommended range. 5. If chatter occurs, reduce depth-of-cut and repeat cut until a successful depth is found. 6. If the tool fails, back off on either the speeds or feeds, depending on the type of failure. 7. Repeat above cuts at 50 percent width of cut. Sometimes a tool that will not slot effectively will machine at 50 percent width of cut very nicely. 8. As tests are run, record the above results regularly. 9. Review cuts and figure out what depth-of-cut and feed/speed combination yields the highest metal removal rate (or best quality of part if that is different). 10. Apply these results on the next part(s) processed.
Did you find this material interesting? Do you want more information of this type? Comment via FEEDBACK
Source: Tooling & Production - Copyright Nelson Publishing Jul 2002
Please patronize our many sponsors, affiliates and advertisers today so that we may bring you more advanced services tomorrow. Have you seen the great deals from top brand name manufacturers?
|
|
|
