For more information on cutting speeds, be sure to download the Waterjet Web Reference Calculator. This calculator will give you a good idea of how thickness affects speed, as well as the cutting rates for various materials. Note, however, that because cutting speed is also a function of the geometry of the part, this calculator is only good for linear speeds.
To design a part for fast machining, you should understand the main factors that affect cutting speed:
- Cutting horsepower of the pump
- Material that you wish to machine
- Thickness of the material you wish to machine
- Geometry of the part
- Type of pierce
- Desired surface finish and tolerance
Simply put, the more horsepower that makes it to the nozzle, the faster you will cut. However, a faster cut does not necessarily translate into a cheaper part. Cutting at higher pressures increases wear on the components of the waterjet and means that you will need to replace them sooner, and rebuild your pump sooner.
As you might expect, each material has a different speed for ideal machining. These speeds are hardly at all related to the speeds that other traditional machines would use. For example, Hastalloy, Inconel, Hardened tool steel, and Titanium all are fairly difficult to machine on most other machinery. With an abrasivejet, however, all of the above materials machine at close to the same speed as mild steel. In fact, titanium even cuts faster.
If you have a choice of material for your part, you should check to see what the waterjet machining times are, and not rely on your experience with other machining methods.
Cutting speed is an exponential function of material thickness. More precisely:
The speed of cutting is proportional to one over the thickness raised to the power of 1.15
This means parts under 0.5″ (1.3 cm) thick will machine quite quickly, while parts greater than 1″ (2.5 cm) thick are much slower. Over 2″ (5 cm) thick, and many shapes are not practical, unless you are roughing out the part, or you can’t do it any other way. In some cases, though, it may be practical to cut much thicker, like 8″ (20 cm) or even more, but it’s rare.
5″ (13 cm) thick slug machined from the center of a very heavy chunk of steel by Cutting Technology, Inc.
The part shown above took about nine hours to make. Generally speaking, it is better to stick to thicknesses of less than 2″ (5 cm). Notice the use of rounded corners to speed things up.
Geometry of the part
Simply put: avoid sharp corners to speed things up. There is nothing wrong with wanting a sharp corner, but if you don’t need one, don’t draw one. Tight curves will also slow the process down. This is especially true of inside corners.
Profile of a toy boat
In the above illustration, colors represent the various feed rates required to obtain a reasonable tolerance, with blue the slowest and yellow the fastest. Notice how much it slows for sharp corners (blue) verses the fast feed rates used on the straight-aways (yellow).
The sharper the corner, the more the machine must slow down in order to maintain tolerance. Therefore, if you want to make the part quickly, avoid sharp corners. On internal corners, you will not only cut the part faster, but you may also be able to hold tighter tolerances.
- All sharp corners will slow the cutting processes down. On thin parts, this is not very important, but on thicker parts the effect is huge.
- Sharp inside corners are hard to hold tolerance in. Some controllers are better than others at this, but expect lower tolerances on inside corners from any machine.
- Sharp outside corners are sometimes faster than radii, if the path is optimized for them. When you get a quote, let them know if outside corners have to be sharp or round, or if it does not matter. If it does not matter, then the operator can use whichever type of corner will be fastest for their controller. Most likely that will be a rounded corner, but it may be square if their controller has the right optimization software for it.
- Fillet inside corners with the largest radius that you can. The larger the radius, the faster it can be machined.
Type of pierce
It takes time to pierce the material. If you have lots of room inside of the scrap material, then faster pierce techniques can be used. If you have less room, then slower pierce methods must be used to fit.
Number of pierces
On and off transitions take additional time and cause fatigue on high pressure components from the pressure fluctuations in the lines. They are also the most likely spot where the nozzle might plug or otherwise cause the operator problems. Having a lot of pierces will slow down machining. If you are machining glass, or another very brittle material, try to avoid piercing as much as possible. Brittle materials can be pierced, but sometimes the glass will crack.
Desired surface finish and tolerance
The smoother the surface finish you want, the longer you have to wait for it. Smooth surface finish is obtained by slowing down the cutting rate. Higher tolerance parts also take longer to machine for similar reasons. Do not specify a higher tolerance or surface finish than you really need.
While it is true that high tolerance parts are typically machined at a slower rate than low tolerance parts, it is not true that the slower you go, the higher the tolerance you get. In fact, after a point, if you go slower, you simply get more taper, and thus less precision. There is an optimal speed for each material and thickness that gives you the best tolerance.
Common line cutting
Common line cutting refers to using one cut to create the edge of two different parts. Imagine that you need to cut a series of rectangular bars from a plate. You could arrange them so that the right edge of one bar is the left edge of the next bar, effectively halving the amount of time to cut that section of the part.
It is often a brain-twister to make an efficient path where some features are common line cut. In addition, the accuracy of the parts will suffer because it is difficult to compensate for the kerf width of the jet precisely without re-creating the tool path as the nozzle wears. Common line cutting is also not practical when using tilting cutting heads for removing taper, since the taper will be removed from one side, but added to the other. It is perfectly reasonable to do common line cutting for low-precision production work.