IntroductionI learned the basics of using a metal lathe while attending high school, in the "metal shops" course, which was part of the "industrial arts" curriculum. In fact, I made one of my first rocket nozzles using a school lathe, with guidance from my shops teacher who taught me how to carry out the more difficult aspects of latheing, such as boring out the interior cone. Some years later, my brother purchased a small metal lathe for our home workshop, a compact Austrian made Edelstaal model with a 10 inch swing, and 24 inches between centres. Using this machine, I progressively improved my machining skills and successfully produced a number of nozzles such as those for the A-100 , B-200 and C-400 motors. I've used this same lathe, in more recent times, to produce the Kappa nozzle, which was later used for the Cirrus One rocket. A few years back I purchased a metal lathe for my own workshop, a medium sized Chinese made Craftex model, with a 12 inch swing, also 24 inch between centres. Being larger, and having a more powerful motor, as well as power cross-feed, makes for more expedient work of producing a nozzle. The largest nozzle I've made to date is that for the 75 mm Lambda motor. All the nozzles that I have produced have been made on a manual lathe, with one exception. While attending University, I had the opportunity to program and run a small CNC lathe to make an experimental "cubic" nozzle featuring a well-rounded internal profile. Made for the B-200 motor, it was static fired to compare the performance with a standard "conical" profiled nozzle. This study formed part of my graduation thesis.
Without a doubt, machining a rocket nozzle is a challenge, especially for those who have had limited experience in metal working. Machining a nozzle draws upon some of the more difficult aspects of lathe use, owing to the rather complex shape and need for accuracy, combined with the desire of producing a lightweight nozzle having all or most excess material cut away. Machining a nozzle is time consuming, especially if using a small lathe to make a large nozzle. For example, the Kappa nozzle took me 18 hours of machining time. More recently, with improved techniques, greater experience under my belt and a larger lathe, an average size nozzle can be completed in 4 or 5 hours.
Still, I'm very much an "amateur machinist". Much of what I have learned regarding latheing techniques have been gained from hands-on experience, from experimenting with different machining techniques, from books, and, unavoidably, from making mistakes. The process of nozzle machining presented here is a compilation (or perhaps distillation) of this experience, using methods that work reasonably well for me. There are undoubtedly variations that can be used successfully and as such, what is presented should be taken more as a guideline than as a set methodology. The means of "best" producing a nozzle is sure to be one of continuing evolution for each individual, including myself. One should feel free to experiment and any suggestions for improvements or simplifications are always welcome.
Materials for Rocket NozzlesThe nozzle represents a key part of a rocket motor. This component serves to accelerate a voluminous mass of stationary combustion gases to supersonic velocities within a very short distance, and in doing so, produces useful thrust. In accomplishing this remarkable feat, a nozzle is subjected to very high pressures, and rapid, dense gas flow at high temperatures. As such, a nozzle must be fabricated from a material that will be capable of withstanding such conditions of structural and thermal loading. As well, any restrictions to the free flow of gases must be minimized, which necessitates a smooth, suitably profiled flow surface. Considering the effort and time invested in making such a nozzle, multiple usage is obviously desired. Fortunately, ordinary (mild) steel is well suited to this application, at least, for many popular amateur propellants. Mild steel machines relatively well. Either "hot rolled" or "cold rolled" steel may be used. Hot rolled is softer and as such cuts more readily. Cold rolled tends to produce a better surface finish with less effort and produces less problematic chips, or swarf. I usually use AISI 1018 steel, perhaps the most readily available grade.
One possible alternative is "Ledloy" (12L14) which is a steel alloyed with a small percentage of lead. I've recently tried machining a nozzle with this steel, and it cuts like a dream. Perhaps the nicest aspect of machining ledloy is that the swarf is in the form of chips which fall away from the cutting tool, as opposed to the long "thready" swarf that mild steel (such as 1018) forms. I have not, to date, fired a motor with this nozzle, so the issue of heat resistance is still an open one. Ledloy is readily available, but may cost slightly more than regular steel. Another alternative is stainless steel. Both alternatives should be used with caution as these alloys may be less resistant to high temperatures than mild steel. Alloy steel such as 4130 should not be used, due to its lower melting point and difficulty in machining.
Update: May 29/05
The nozzle for the Liberty "L-class" rocket motor was recently machined from 12L14 steel. The intent was to reduce the labour required to machine this rather large nozzle, and this was very much the case. After three firings, the nozzle showed zero throat erosion, so the capability of 12L14 steel to stand up to the heat of combustion has been confirmed.
An alternate non-metal material that is especially suitable is graphite, although the use of this material requires special considerations, due to the copious amount of messy and electrically conductive dust that is generated. An old shop-vac with a very fine dust filter works well to draw away the dust as it is produced. Graphite nozzles are ideal for use with high combustion temperature propellants such as APCP, for which steel is not suitable.
Low melting point alloys such as aluminum and brass are not suitable for multi-usage nozzles, unless a high temperature resistant "throat inset" is used (which complicates the manufacturing). This technique has been used with good success for Hendrik Lau's HL6000M rocket motor. The nozzle is fabricated from aluminum alloy and features a high-density graphite insert (see Appendix D for photos).
Use of BlueprintsIt is, of course, quite feasible to make a nozzle "on the fly" without need of an engineering drawing, commonly referred to as a "blueprint". However, the more rational approach to rocket motor design and construction involves designing a nozzle to achieve a particular performance goal. This design process defines the nozzle shape and dimensions. Key design parameters for a standard conical deLaval nozzle are the convergent and divergent angles, and the diameters of the inlet, throat, and exit. As well, the exterior profile of the nozzle is sculpted to minimize the mass of the finished nozzle. A nozzle that does not have a sculpted exterior will work nearly as well. However, if it is made of steel, it will be heavy! Graphite nozzles do not require much or any sculpting of the outer profile, as graphite is very lightweight, having approximately half the density of aluminum. Other design details include determining the diameter of that portion of the nozzle that interfaces with the casing, and o-ring groove dimensions and location. Additionally, the means of attachment to the motor casing, which will typically be machine screws or snap rings. It is important to recognize that the more care and effort that is put into creating an accurate and detailed blueprint, the less laborious the effort to fabricate the nozzle and the less likelihood of making a mistake during machining which could relegate hours of effort to the scrap bin. CAD software programs (even basic ones) are ideal for producing a suitable nozzle drawing. I use QuickCAD, which I find to be easy to use, powerful and relatively inexpensive. Freeware,"Shareware" or free-trial CAD programs are also available. Alternatively, scaled drawings may be made the old-fashioned way, by hand.
Tools requiredIn addition to a metal lathe and basic cutting bits such as those required for the turning and facing operations, a few other tools are needed for nozzle making. Boring bits are needed for cutting the interior convergent and divergent profiles of the nozzle. For machining nozzles with a small throat diameter, such as the A-100, it will likely be necessary to custom-make a boring tool, as commercial boring tools are generally too large to permit boring of such small hole diameters. A parting tool bit and holder is needed for cutting o-ring grooves and snap-ring grooves. A tailstock mounted drill chuck is also required, as well as drill bits. These are needed for drilling out the throat and for initial material removal of the convergent and diverent cones. A special short, stubby drill bit called a centre bit is required to ensure that the drilled hole is perfectly concentric (regular twist drill bits are too flexible). A hacksaw, bandsaw or friction blade is needed to cut the steel bar to length. One other tool is essential - a good quality dial caliper (or digital caliper) gauge, used for precision measuring. Other tools that are useful but not essential are a depth gauge and bore gauges.
Three custom made boring bits suitable for machining nozzles with small diameter throats are described in Appendix A.
Latheing ProcessesMachining a nozzle involves six cutting operations inherent to latheing: facing, tapering, turning, boring, drilling and parting.
The first four of these, as well as other latheing operations, are shown below in Figure 3.
Facing is used for truing the ends of the workpiece and to trim the workpiece to the required length. Tapering is the operation that forms the outer profile of the nozzle divergent cone, and is performed by rotating the compound-slide at the angle required to produce the divergent cones. Turning is the operation that cuts parallel to the workpiece axis and serves to reduce the diameter of the workpiece. Boring is an operation that shapes the interior profile of the nozzle, and is the trickiest and most time consuming process. However, much of the boring can be eliminated by first "step drilling" the workpiece to the approximate profile of the interior, then employing the boring operation for the final finishing cuts. The parting operation is used solely for creating the o-ring or snap-ring grooves, and as such, is not a true parting process. However, the basic concept is the same.
Another machining process that I've recently experimented with in regard ot nozzle fabrication is reaming. A reamer is a tapered cutting bit that can be used to machine the profile of the convergent or divergent cones. The use of a reamer is discussed in Appendix B.
It is highly suggested to review the links provided in Appendix B to become more acquainted with the construction and terminology of a metal lathe, as well as the various machining operations.
General Latheing TipsUsing the correct cutting speed is important in order to avoid "chatter" and to avoid overheating the tool bit (with resultant premature dulling). A higher cutting speed can be used with carbide bits. For basic cutting operations such as turning or facing, a good surface cutting speed for AISI 1018 steel is 130 fpm (ft. per minute) for HSS bits, 1.5 to 2 times that for carbide bits. Ledloy 12L14 steel reportedly can be cut at 325 fpm with HSS bits. Table 1 correlates surface cutting speed to workpiece diameter and RPM.
Example: A nozzle is being machined from 1 inch diameter cold rolled 1018 steel using a HSS cutting bit. As such, a cutting speed of 130 fpm will be used. From Table 1, the RPM should then be set for 479 RPM (or thereabouts).
Feed rate of the cutting bit , and depth of cut, are also important. Feed rate is the linear speed at which the cutting tool is fed along the workpiece; depth of cut is how much material is removed with each pass of the tool bit. Basic cutting operations such as turning can tolerate a greater feed rate or cutting depth than the more delicate operations such as boring. For turning, the ideal cutting rate should produce swarf that gets hot enough to produce a straw-yellow oxidation coating. Blue coloured swarf indicates too high a cutting rate. Lighter cutting rates are fine, but extends the overall time required to fabricate a nozzle. Here is a photo of some first-rate swarf from a boring operation.
Cutting oil (coolant) should be used with HSS (High Speed Steel) tool bits. I use water-soluble coolant, mainly because it cleans up more readily, is odourless and is smokeless. Use plenty of cutting oil when drilling and tapping. Tungsten carbide bits should be used without coolant. Both HSS and carbide bits should be sharpened regularly. This will noticeably ease the cutting operation as well as provide for a better surface finish. Carbide dulls at a much slower rate, however, the cutting edge will gradually deteriorate. For HSS bits, use a regular aluminum oxide wheel for sharpening. For tungsten carbide, a green silicone carbide grinding wheel works well (do not use for HSS bits).
Machining the NozzleThe basic steps that I follow for the machining of a nozzle are given below.
Machining GraphiteDue to its high temperature capabilities, graphite is an excellent material for rocket nozzles, especially for hot burning propellants. Two drawbacks are graphite's relatively low strength and brittle nature. Graphite stock is also quite a bit more expensive than metal stock. For these reasons, graphite is usually used to make a throat insert, rather than a complete nozzle. Figure 14 illustrates a graphite throat insert. Inserts are fitted into a metal nozzle shell, usually as a tapered plug fit.
My experience with machining graphite is fairly limited, and is on-going. What follows is based on this limited experience. Graphite machines well, and larger cuts can be made compared to metal. However, graphite stock is an abrasive material, and tool bits tend to dull rather quickly. Although graphite is a natural lubricant, apparently it is the binder that gives graphite stock an abrasive nature. Since dull tool bits affect accuracy of a cut and the quality of the finish, bits should be re-sharpened frequently. For this reason, tungsten carbide is a better choice than HSS. In industry, diamond coated tool bits are sometimes used to machine graphite stock to extend tool life and for reduced cutting friction.
The cutting operation produces tiny chips accompanied by a very fine dust. The dust is quite pervasive, and besides making a mess, can damage electric motors and switches due to its electrical conductivity. As such, it is paramount to control the dust. The method I use is to vacuum up the dust as it comes off the cutting bit, using a wet/dry shop vac. This particular vacuum cleaner has a high-capacity, multi-pleated filter that can tolerate a large intake of fine dust without impeding air flow. As well, the removable pleated filter can be readily cleaned. An even better solution to dust capture may be a disposable dust bag that fits over the pleated filter. Such bags are available for many shop vacs.
I devised a simple solution to avoid having to manipulate an unwieldy vacuum hose and crevice tool around the cutting action. A length of 3/8 inch (ID) flexible vinyl tubing is simply inserted into the mouth of the crevice tool (do not further block the intake, as the vacuum motor requires unimpeded air flow for cooling!). The other end of the tubing is then placed near the cutting action for dust pickup. The tubing can be conveniently taped or tie-wrapped to the toolpost, or manipulated by hand. This solution works well to suck up the fine dust. The larger chips fall into the lathe bed for later cleanup.
Graphite chips should be thoroughly cleaned from the lathe components because of the potential for wear of moving parts (e.g. ways, feed-screw) due to the abrasive nature of the chips. Graphite dust that gets on your hands, or on the floor, cleans up well with soap (an effective emulsifier) and warm water.
Graphite stock is usually cut dry. Oil-based lubricant should not be used (messy). I have heard of water being used to keep down the dust, however, I would not recommend this due to the potential for rusting of the lathe parts.
The cutting bit should be ground with a zero rake angle to reduce flaking and consequently improve surface finish quality.
Appendix ACustom-made boring tools
I. If the throat diameter of the nozzle is quite small, such that a standard boring tool can't quite get into the confined space, it is often possible to modify the tool bit such that it can accomplish the job. It is simply a matter of sculpting the tool bit around the cutting edges to remove excess material in order to give the needed clearance. This is done using a power grinder. It is important to prevent the cutting edges of the bit from getting hot. As such, the bit should be regularly dipped into a pan of water. To make certain enough material has been sculpted away, position the tool bit into the nozzle near the throat, and inspect closely for interference. As well as removing material from the sides of the bit, grind the bottom surface, especially at the front end of the tool bit.
II. Several years ago, after realizing that the boring tool that I was using to make a nozzle was simply too big to machine the throat region (even when all excess material around the cutting edges was ground away), I searched the workshop for something to make a small boring tool from. I came across an old, small flat file, roughly ½" wide by 1/8" thick. Perfect. I carefully ground away the tip to reduce the width, and improvised cutting edges. I found that this tool worked well, and used it to successfully machine the finishing cuts of the nozzle where the standard boring tool could not reach. The only major drawback with this tool, being of carbon steel rather than HSS, is that it tends to need resharpening often (thereby shortening its useful life).
III. More recently, while fabricating a nozzle for the new A-100M motor, I decided to try to make a boring tool using a HSS tool blank, which should be capable of keeping a sharp edge for a longer time. I had recently purchased some small 1/8" square blanks, just about the perfect size for boring the ¼" diameter throat. To hold the tool bit, I utilized a length of 3/8" hex steel bar, into which a suitable diameter hole was drilled. Into this hole, the bit could be inserted with a snug fit. To prevent rotation of the bit, I drilled & tapped two holes and installed #6-32 Allan (set) screws. Cutting edges were added and excess material ground away from the tip to maximize clearance when cutting in the confined region at the throat. This boring tool was found to work very effectively.
Left: Sculpted boring tool bit, compared to a similar "as purchased" tool bit.
As an alternative to boring, a tapered reamer can be used to cut the inner profile of the nozzle divergent cone. A tapered reamer is a cutting tool bit that has tapered cutting edges. Reamers, which are made from HSS, can be quite expensive, especially for the larger sized ones that are suitable for nozzle work. I happened to come across such a reamer during a recent visit to Princess Auto & Machinery, which specializes in surplus tools and machine parts, that was affordably priced ($20 CAD). This particular reamer has a 7.5o half-angle, which is quite a lot more shallow than the conventional 12o half-angle that I usually use for my divergent cones. The main drawback to such a shallow angle is the increase in nozzle length, and therefore weight, that results.
I have experimented with using this reamer on steel nozzles and on graphite nozzles. For graphite nozzles, it works exceptionally well. It is only necesary to cut a pilot hole through the length of the nozzle, then use the reamer to enlarge the hole and form the tapered divergent cone. This process is illustrated in the photo below.
For a steel nozzle, it is necessary to use the method described earlier of drilling increasingly larger holes to create a "stepped" profile. This serves to remove most of the material. The reamer is then used to finish cutting the divergent cone. I have found that the reamer works very well, with essentially no chatter or other difficulties. Plenty of coolant is used to help maintain the tool's sharp cutting edges.
Appendix CUseful Links
Virtual Machine Shop - A must-see site, includes video clips explaining parts of the lathe and various machining operations : Engine Lathe - Topics
Appendix DSome of the rocket nozzles I have machined
Hendrik Lau's HL6000M aluminum alloy nozzle with graphite insert
Sugar Shot to Space project:
Tapping (threading) holes for installation of machine screws is a common and simple operation. Nevertheless, a tapping bit will occasionally break during tapping, despite care being taken. Not only is a broken tap an aggravating occurance, it can be quite problematic. This is especially true if the workpiece represents a large investment in time and effort. An excellent example is a rocket nozzle. I have experienced this mishap on occasion despite my awareness and best efforts at careful tapping. The smaller the tap size the more vulnerable it is to breakage, especially when tapping a harder material such as steel. Taps larger than #10 screw size are not readily broken. I have learned to be particularly careful when tapping small holes by minimizing applied torque and by avoiding any bending that could overstress a tapping bit. Nevertheless, I have experienced breakage even when administering such care. My own theory is that the breakage is often a result of metal fatigue, that which is known as "low-cycle fatigue". A product of unavoidably high stress, stress concentration and tiny intrinsic flaws in the bit, low-cycle fatigue can lead to microscopic crack growth followed by sudden breakage even while being lightly loaded. I have noticed a correlation between such breakage and amount of usage a tapping bit has undergone.