CNC milling toolpath optimisation has been around for a while, but there has been a recent spurt of activity from CADC AM vendors. Andrew Allcock reviews recent happenings, reveals why and gets into the detail
CNC toolpath optimisation can mean a number of things, including the elimination of fresh air cutting or taking the shortest cutter path. But recent activity, and Machinery's main focus, is the optimisation of cutter/material engagement within a CAM system to deliver maximum/consistent cut volume or consistent cutter load or chip thickness - and 'feedrate optimisation' or 'adaptive feedrate' as a post-CAM operation where output NC code is modified.
Within that broad classification, there are further differentiators, such as whether the technology supports 3D contoured toolpaths or 2½-axis cutting (X-Y moves at different Z depths), and whether roughing or both roughing and finishing are supported.
Key claimed benefits for toolpath and feedrate optimisation are reduced cycle times, improved tool life, improved surface quality and reduced machine tool wear.
At the International Manufacturing Technology Show (IMTS) in Chicago, USA, last September, the technology was prominently highlighted by three machine tool makers. All were employing American company Surfware's TrueMill technology (www.surfware.com
), applied within its Surfcam CADCAM system to generate optimised roughing cuts for 2½-axis machining. The three machine tool companies that made it part of their IMTS exhibition demonstration were Okuma (NCMT, 020 8398 4277), Hardinge (0116 286 9900) and MAG (0121 306 5600).
For Okuma, the focus was on demonstrating that smaller machines employing TrueMill-generated toolpaths can deliver benefits, even when tackling titanium. The company's new compact, high speed Millac-44H - a 320 mm diameter table horizontal machining centre with 8.2 kW spindle and Okuma OSP/THINC CNC - was shown machining 6AL4V titanium at a rate of over 4.5 m/min, using a 12 mm diameter end mill, working at a 25 mm depth of cut: it achieved peak material removal rates of almost 100 cm3/min. In parallel, improved tool life was also highlighted.
On Hardinge's stand, the company's new Bridgeport GX-1000 OSP VMC (1,000 mm in X-axis) - also fitted with Okuma OSP/THINC CNC - was cutting alloy steel 4140. The machine was shown cutting at over 12 m/min, using a 12 mm diameter end mill at 25 mm depth of cut, achieving peak material removal rates of 305 cm3/min.
Finally, MAG used TrueMill technology in combination with its new 16-flute Cyclo Cut Max-Flute high performance end mills to tackle titanium milling, demonstrating high volume cutting at low torque levels. The end mills, run at 2,037 rpm and set to cut at almost 5.9 m/min, supported a material removal figure of 131 cm3/min.
Surfware's TrueMill began life in 2002, so has been around a while. It is the subject of US patents and is described by the company as "a quantum leap in CAM toolpath technology". The technology's key factor is that it maintains a constant engagement angle between tool and the material being cut to maximise the material removal rate (MRR). This eliminates, for example, dramatic increases in tool engagement when tools enter corners in pockets by producing novel toolpaths, rather than modifying 'traditional' toolpaths. Indeed, Surfware CEO Alan Diehl offers this: "Toolpath optimisers [that work on NC code] are not capable of taking an existing conventional toolpath and modifying it, so as to achieve constant engagement."
Image: Cutter engagement is at the heart of TrueMill's technology - 120 degrees, good
Image: Cutter engagement is at the heart of TrueMill's technology - 165 degrees, bad
Image: TrueMill delivers novel toolpaths
Image: Traditional toolpaths for a pocket - offsetting from the basic geometry
The only variation to the application of constant engagement angle is, highlights Mr Diehl, in 'corner picking' or areas where it is not possible, with a conventional tool path, to machine the corner without exceeding engagement. Here, several tool passes of decreasing radii are arranged, such that engagement is not exceeded while machining each pass. This process allows machining corner radii only 10% larger than the tool radius without exceeding engagement.
And he underlines why optimisation of TrueMill toolpaths is unnecessary: "Toolpaths are generated by an algorithm that takes into account the shape of the region to be machined and the engagement angle, generating a toolpath that maintains both engagement and the actual maximum undeformed chip thickness (not the 'chip load') throughout the toolpath. Because the toolpath is created for the region to be machined 'toolpath optimisation' is not required. In addition, since engagement is controlled, a constant feed rate generates a constant material removal rate. The tool always 'sees' the same cutting conditions."
The company's public claim is that: "TrueMill allows a cut that is both faster and deeper than any other 2 or 3-axis roughing toolpath on the market today. TrueMill is the only toolpath engine that manages tool engagement to significantly increase productivity."
The clue to why the technology, after almost eight years of being, is now attracting attention is that challenging aerospace alloys are being machined more and more. Surfware's Peter Marton told Machinery: "Yes, the message of 'tool engagement' milling is finally catching on in the machining world and machine and cutting tool companies love it.
"The benefits of TrueMill are now being realised in the market, now that the cutting of titanium and hard metals is coming to the fore. The more difficult the materials being cut, the better TrueMill works."
According to Surfware, TrueMill toolpaths have been proven to increase material removal rates by up to 10x and increase tool life anywhere from 30% to 100%, while at the same time decreasing cycle times and reducing the stress on CNC machines. (In 2010, Surfware developed a TrueMill business and the technology will soon be available for licence to other CADCAM companies.)
Vericut CNC toolpath simulation software (CGTech, 01273 773538) is another software package that has had toolpath optimisation as an optional element for many years - OptiPath. Vericut is not a CAM system, but is instead used to review and check actual CNC G-code generated by CAM systems, including 3D contouring paths, which Optipath also supports.
Image: Vericut offers 3D toolpath optimisation
UK agent CGTech's managing director, John Reed, suggests Vericut has an advantage over CADCAM systems. "The key issue is that Vericut produces a constantly updated in-process cut model and, therefore, has the information about the tool and the part used to calculate constant volume and chip thickness cutting. This in-process cut model is not available in CAM systems – it is a bi-product of the simulation process."
And he questions how the calculations are being performed within CAM systems concurrent with toolpath generation. Responding for Surfware, Mr Diehl highlights that Mr Reed is correct in respect of 3D contouring toolpaths, but that "it is not true for 2D or 2 1/2 D machining, where the cuts are made at various Z levels", he explains further.
Returning to Vericut's OptiPath, this modifies existing 'traditional' toolpaths for roughing and finishing. Through the simulation process, it is said OptiPath learns the exact depth, width, and angle of each cut. It knows exactly how much material is removed by each cut segment and, with that knowledge, it divides the motion into smaller segments. Where necessary, based on the amount of material removed in each segment, it assigns the best feedrate for each cutting condition encountered. It then outputs a new toolpath, identical to the original, but with improved feedrates. It does not alter the trajectory, it is emphasised.
During roughing, the goal is to remove as much material, as quickly as possible. Here, OptiPath keeps the cutter at its maximum safe rate-of-advance into material for the varying cutting conditions.
When it comes to finishing, chip loads typically vary widely, as the tool profiles through the material left behind during roughing cuts and over the contours of the workpiece to near net shape. OptiPath adjusts the feedrates to maintain a constant chip load - consistent chip loads are recommended by cutting tool makers to reduce 'chip thinning' - with the result that tool life and surface finish are improved.
Like Surfcam, Mr Reed agrees that the benefits of such optimisation are magnified when machining challenging materials. "The biggest bang for the buck is certainly with roughing, and hard-to-machine materials like titanium see a particular benefit because they take a long time to machine. And even if the percentage reduction isn't so great, you can still save large amount of time, because machining times are so long. Additionally, maintaining constant chip thickness really helps when you cutting something like titanium."
But machining complex shapes using 5-axis machines, regardless of material, is also cited as an area of beneficial application.
"What people tend to do, to avoid cutters diving in to material as geometry changes, is to program for the worst-case scenario, which obviously gives problems. Conversely, people using OptiPath don't worry about the lateral feedrate; they put a really high one, because they know OptiPath will reduce it."
CGTech's managing director says that it has been "frustrating" trying to get people interested in this particular Vericut capability "because the potential for it is great". The problem, he says, is that optimisation is seen as yet another process between programming and machining – effectively another Vericut simulation pass. Additionally, if work is not of a repeat nature, people say they don't have time, he adds. "This doesn't really make sense because some of the savings are quite substantial. And for those that have repeat batches, they have saved so much time they actually avoided the need to invest in additional machines," offers Mr Reed.
Indeed, those that are using the process are not necessarily keen to boast of their success, he says, because the time savings are so great that they want to maintain the whole benefit for themselves and not, for example, get into new pricing discussions with customers. There is one quote used in the company's promotional material, though. "Four-and-a-half hours of programmer time spent on optimisation saved us $75,000," according to Brian Carlson, programming manager, Aerospace Dynamics International, USA.
But the good thing, offers Mr Reed, is that at least people are beginning to think more about this area. "In the past, people hadn't thought about it and just used the worst-case scenario, thinking that 'maybe we can tweak it once it's in production and proven'. It's pretty unscientific, isn't it?" he muses.
However, speaking for Edgecam (0118 975 6084), strategic product director Raf Lobato suggests that the post-CAM optimisation of toolpaths is really an admission of poor strategies within the CAM system. "It is a failing when a toolpath that comes out needs optimising: it is the wrong place to do it, because you have lost all associatively with the CAD model, while it is just addressing weaknesses in a CAM system.
"I used such a product on a toolpath not generated by Edgecam and got a 30% cycle time improvement. However, we remodelled the toolpath within Edgecam and, low and behold, discovered the program was using the wrong diameter tool. It was machining a large pocket with small corners, using the cutter that suited the corner radius. By using a roughing and rest roughing strategy in Edgecam - so a large diameter cutter, followed by a smaller diameter cutter - the time saving wasn't 30%, it was nearer 75%.
"Optimising afterwards does have benefits, but it's a bit like souping up your car and driving faster down a country road, while ignoring the motorway alongside on which you could be travelling even faster." And Mr Lobato adds that, when applied to Edgecam toolpaths, the improvements are "minimal".
"Additionally, CAM output must also take account of the machine control," he says. "Some modern ones will want output in the form of many small G01 moves (straight line moves), older controls cannot cope, so we can offer output options such as arcs or even NURBS. Without the data appearing at the machine tool in the correct format, any optimisation might be wasted, if the machine can't keep up with the data flow," he adds.
Edgecam has, for many years, taken a roughing approach that offered a constant chip load, using, for example, lacing patterns and concentric patterns, explains Mr Lobato. A drawback is that cutter overload could arise, so things like S-links between toolpaths and spiralling between concentric toolpaths were introduced to minimise that, while an ability to slow the feedrate down was also added – all of this was done many years ago, it is emphasised. More recently, trochoidal toolpaths (small spiralling toolpaths) were developed in conjunction with Sandvik Coromant (0121 504 5400).
"So today, the user can choose whether to slow the feedrate down or introduce trochoidal milling into any toolpath, and can use lace, concentric or spiral patterns," explains Mr Lobato. But the company is about to unveil a new strategy, Wave Form. This supports constant chip load (constant volume) 2½ axis milling, so that feedrate can remain constant. Wave Form removes the need for adaptive feedrate and trochoidal milling approaches, and it will result in novel-shaped toolpaths that are not a simple offset of the shape of the final geometry, in similar vein to TrueMill. The technology has been developed with Sandvik Coromant to obtain best entry and exit paths, while eliminating repeated entry and exit that blunts the tool - a weakness of trochoidal milling. "In this area, we believe we have leapfrogged the competition," says Mr Lobato.
Image: Edgecam Wave - produces novel toolpaths, like TrueMill
The choice of Wave Form or any other roughing strategy will be available to users at the click of a mouse, with them able to see which one delivers the best cycle time, too.
The major benefit will be on hard materials and he suggests a 35% improvement over existing roughing cycle times "is not unrealistic", assuming machine and cutter technology that is able to exploit Wave Form. For softer materials, 'traditional' strategies may be better because the novel toolpaths are not short, and if the machine cannot travel much faster than it is already is, clearly cycle time will be negatively impacted, it is stressed.
To maximise metal removal, large depths of cut are used, so to minimise large steps across a 3D surface so-called Intermediate Slices Technology, which already exists, is employed as a secondary process to reduce these steps, it is explained.
Two recent members of the toolpath optimisation club are CADCAM companies Delcam (0121 766 5544) and Open Mind Technologies (01865 338026). Open Mind's offering is hyperMAXX, a roughing strategy powered by the established Volumill toolpath engine from America's Celeritive Technologies, a company set up by ex-Surfware personnel, in fact. (GibbsCAM (Tech CADCAM, 01284 754781), Mastercam (4D Engineering, 01285 650111, Esprit (Cam Supplies & Services, 0871 218 3001) and Sigmanest (SigmaTEK Europe, 024 7632 3065) can also employ Volumill technology, although it may not necessarily be integrated within the package - see http://bit.ly/feEs1Z for a GibbsCAM case study.)
FIRST CUT IS THE DEEPEST
Volumill is, like Truemill, a technology for 2½D rough machining, producing 'novel' toolpaths. (Full Volumill Q&A here - http://bit.ly/haLhvl). But while it does not support 3D contouring, it does support machining of 3D geometry at multiple Z levels via use of two, distinct depths of cut within the same toolpath.
First, deep axial cuts, up to the full flute-length of the tool, can be used to remove the bulk of the material as quickly as possible. A second, smaller depth of cut can also be set to leave a perfectly uniform, user-specified final step height on the model. This approach is said to minimise roughing and overall cycle times, machining the part to a near-net shape, and requiring the use of fewer tools. Surfware offers a similar approach, called Step Reduction Milling (patented), which is combined with TrueMill. Edgecam's Intermediate Slices Technology is also clearly similar.
Volumill has two other cutting strategies: 'opening cut', suited for full cut machining of areas that are difficult to reach and effective in softer materials, such as aluminium; and 'side cutting only', which sees lateral in-feed movements, without full cutting, designed for machining harder materials. Open Mind claims that roughing time savings of 50% or more are typical with hyperMAXX.
Image: Open Mind's HyperMAXX uses Volumill technology - adaptive feedrates show here
Image: HyperMAXX - Opening Cut
Image: HyperMAXX - Side Cut
Delcam's technology supports both rough and finish cutting, plus it accommodates 3D contoured surfaces. The optimisation capability is a feature of the 2011 version of its PowerMILL CAM system for 5-axis and high speed machining. Key is the new stock-model-engagement option.
A number of CAM programs incorporate strategies based on the extent of cutter engagement to give more consistent loading on the tool and so allow higher feedrates, explains Delcam, but these options are "usually limited to the initial roughing operations, or to only roughing and rest-roughing". PowerMILL's new stock engagement technology can additionally be employed with all of the CAM system's finishing and rest-finishing strategies, it is said.
Image: Delcam's PowerMILL supports both roughing and finishing - it employs a stock model updated in real time
In keeping with CGTech's John Reed's thinking, the company says: "The key to this more comprehensive solution is the accuracy of the stock models produced within PowerMILL after each machining stage has been completed. These models give a precise representation of the material still remaining on the part and are used to ensure that the cutter is never asked to remove more material than it can safely cut." Fresh air cutting is similarly avoided.
Enhancements to feed-rate optimisation have been introduced within PowerMILL to give better control of leads and links at the points of cutter engagement and exit. Typically, the feedrate as the cutter enters and exits the material needs to be slower than that set for the main length of the toolpath. Setting the entry speed too high will risk damage to the cutter and the spindle, and can even move smaller parts on their fixtures. Exit speeds are critical when machining brittle materials, such as graphite electrodes, since the cutter can chip the surface of the part if it is moving too quickly. PowerMILL users can avoid these problems by setting specific entry and exit feed-rates.
So, optimised toolpath generation concurrent with CAM programming or after the event feedrate optimisation, with all this recent development it might be prudent for machinists to revisit this area to glean what benefit there is to be had.
Box item links
 Vero and Sescoi NC code optimisation; FeatureCAM federate optimisation
 NC code optimisation software to compensate for slow CNC units
 CNC adaptive control and Siemens technology
 Further reading
Box item 1
Who else is optimising?
 Both Vero (01242 542040) and Sescoi (01242 542040) employ German company FormTEC GmbH's software
. Vero calls the package NC Optimiser, while Sescoi calls it NC Speed.
The software takes post-processed code and optimises the NC program, based on the volume of material to be removed, delivering a higher average federate – a solid stock model is employed. It supports 3D surface machining, roughing and finishing processes. Machining time reductions of up to 20% are claimed.
NC optimiser adapts the NC program feedrate to match the machining conditions, based on the volume of material to be removed. Using a simulation of the machining process, NC Optimiser determines the load that would be generated in the actual cutting process and compares these values with the tool's user-specified load limit.
In areas with low cutting volume and favourable milling conditions, the feedrate is automatically increased. In critical areas, where additional stock is detected, the feedrate is reduced to prevent costly tool damage and a scrapped work piece. Arcs will be optimised, as well as linear movements.
Importantly, points out Vero, the software doesn't alter, in any way, the source NC file: it will only add strategic new points to the original NC file, in order to smoothly adapt feed transitions.
Typically, mould and die makers, Vero's main customer base, are not under the same productivity constraints as are more production oriented companies, offers Marc Freebrey, group marketing manager. However, in Germany, for example, or in companies where the volume of tooling is very high and that compete on a global scale, NC Optimiser "is a widely excepted solution for all CAM strategies".
Image: NC Optimiser reacts to conditions
Image: NC Optmiser, optimised feedrates - red = fast; blue= slow
Image: NC Optimiser - see the difference?
Image: NC Optimiser - reacting to conditions
 Delcam's FeatureCAM's FeatureMILL software features a feedrate optimisation capability (0121 766 5544). Tool load can vary throughout a toolpath, due to increased depth or width of cut. FeatureMILL2.5D's feedrate optimisation minimises these variations by automatically adjusting federates, based on tool load.
Box item 2
Optimising NC code for older CNCs
US company NW Designs (www.nwdesigns.com
) offers a slightly different type of NC program optimisation, one related to circumventing poor machine processing capability and improving surface finish. It offers MetaCut Finish for 3D machining. President Bill Elliott explains. "MetaCut accurately fits arcs to the point-to-point data produced by your CAM system. One arc often replaces more than nine out of 10 lines with a single arc, even at extremely small tolerances. This means that the physical length of each block is longer. With longer blocks the BPT (Block Processing Time) of the CNC can be much slower without inducing the stuttering or shaking problems caused when the BMT (Block Machining Time) is shorter than the BPT."
Box item 3
Adaptive machining via machine tool CNCs
According to ARC Advisory group's Sal Spada, who wrote an article last year (here
), adaptive machining facilities within CNC controls also offer cycle time, surface and tool life benefits. The article says: "According to recent research, on average, adaptive machining solutions increase productivity by 14%. Most applications are in high production volume aerospace and automotive manufacturing," it continues, saying that cycle time improvements are in the range of 7-15%. Many users also experience a dramatic reduction in tool breakage in their operations, which enables them to consider using more expensive tooling in the production operations, leading to further increased tool life, as well as improved surface finishes.
Siemens, for example, has integrated Israeli company Omative Systems' adaptive control and monitoring software (ACM) for real-time feedrate optimisation, within its controls (www.omative.com). ACM can be used for every cutting operation in feedrate control, monitoring and event-recording modes.
In feedrate-control mode, ACM measures the current spindle load and continuously calculates the optimum feedrate for each individual tool and material. The feedrate is set to the highest possible value, automatically and in real time. This reduces cycle times and also prevents tool breakage and damage to the tool and spindle, particularly during critical roughing operations and in rough-finishing applications. If the tool becomes overloaded, ACM stabilises to an acceptable value automatically. This value is defined via an algorithm in the internal expert system and, if necessary, the feed is suspended. In this way, tool breakage can also be detected.
In monitoring mode, the spindle load is monitored without adaptation of the feedrate. If the spindle becomes underloaded or overloaded, an alarm is triggered and, if necessary, the machine is stopped. Missing tools or tool breakages are also detected.
In event-recording mode, the machine's event data is saved or transferred via the PC network using the Omative Pro software and can be analysed in machine and production reports. Event recording is performed automatically in feedrate-control and monitoring modes.
Omative Systems is currently working on two joint development projects within the European Commission's 7th Framework Program (FP7) that call on its expertise.
One of them is Advanced Intelligent Machine Adaptive Control System (AIMACS), which aims to develop active, self-optimising 'intelligent' Adaptive Control systems that continuously analyse a wide range of monitored machining process parameters, and automatically adapt the machine operation in real time to its optimal performance. It ends in 2013 (see here
Other suppliers of technology to support adaptive control include:
Artis, Germany with its CTM product
Caron Engineering in the USA, with its TMAC product
Digital Way, France, with its WattPilote product
MCU, Germany, with its ToolInspect product
Montronix, US/Germany, with its Spectra product
Box item 4
NC toolpath optimisation – further reading
A 'Google' for information on this subject turns up a page which links to a number of eBooks on the subject. For those wishing to read material of an academic nature, visit http://khup.com/keyword/nc-tool-path-algorithm.html
First published in Machinery, February 2011