Improving the Performance of Your 5-Axis Milling Machine

CRAIG CHESTER: OK, 4:30 it is, so let's kick this off. Just a quick introduction, my name is Craig Chester. My history-- I've kind of been Delcam, then Autodesk, for the last 30 years. During that time, I've really concentrated on the PowerMILL product, and my position today is Product Manager for PowerMILL and, much more recently, Fusion 360, where I'll be concentrating on the milling aspects of Fusion 360.

So I'm guessing there are people in this room who know a lot more than me about Fusion 360 at this moment in time. It's relatively new to me, but that will be a big part of my future. This presentation, we're concentrating on multi-axis machining, and some of the solutions that I will show-- I will be presenting to you the PowerMILL product, how it would provide solutions to some of these problems.

But I think in due course, as a product manager for Fusion, I'll be looking to get some of these solutions. Hopefully we do it better the second time around, but to get some of that stuff into Fusion 360. OK, I had no idea who my audience was so I've done a lit-- just a brief explanation of what 5-Axis is. I know a number of you went to [? Mike ?] [? Caligri's ?] class, so a little bit of this is repetitive.

So 5-axis machining. I preferred Mike's term, actually, multi-axis machining. Why do people want to get involved with it? So some of the big reasons are displayed on the screen, obvious reasons-- fewer setups. Fewer setups saves a lot of time, and money, and fixtures. Shorter, more rigid tooling, much less deflection, less chatter, et cetera, and reduced cycle time-- those are three of the big reasons that people like you will be interested or are already using multi-axis machining.

Mike's images were much better than mine, which is quite upsetting. 5-axis, what does it mean? Well, anybody used to milling knows that we have three linear axes, x, y, and in England we say zed, but I'm going to try and say zee. OK, now on top of that, there are rotary axes. Typically, we will have two of the three, the a-axis rotates around the x-axis, be around y, and c around z.

OK, so on a typical 5-axis machine tool, we've got the three linears and two of the three rotaries. So here's a couple of examples. This machine has a c-axis table. So that's rotating around z. And an a-axis, as we can see, rotating around x.

This next machine, a b-axis on the head rotating around y and a c-axis on the table rotating around z. And then a more unusual machine, where we've got an a- and b-axis. Most 5-axis machines have a or b and c. This machine, Matsuura machine, has an a around x and a b around y.

OK, so let's have a look at some of the configurations of the more popular 5-axis machines, just general categories. We have the table-table machine, two examples on the screen, one with a b- and c-axis and one with an a- and c-axis. The second option is probably one of the most common types of machine called a Trunnion table machine.

OK, so why do people buy this type of machine? Generally, what are some of their positives? Great for undercut machining. Many of the-- excuse me. Many machines with the a,b-axis on the head have a maximum tilt of 90 degrees. That's really common.

With a table machine, typically we're going to get greater than 90 degrees, 110, 115, depending upon the machine type. So we can get into undercut situations. We can point the tool upwards.

Quite commonly, it's only on one side, so we may have plus 30, minus 115, so we're only going to get it on one side of the table quite commonly. Slight difference between these two machines-- the Trunnion table on the right is going to cope with heavier parts better. It's got the two fixing points. And when we've got a real heavy part on there, that part's getting swung about at quite rapid rates, so the Trunnion table generally offers greater rigidity.

The machine on the left, which isn't a Trunnion-- we've got the b-axis rotating around y-- is less rigid but offers more support because we haven't got the upstands of the Trunnion so we can get a larger part on the overhanging the table, so the potential for larger parts on machine A. These machines are good for heavy metal removal. Essentially, the top of the machine is a 3-axis machine, so the spindle is going to be geared or belt driven, which has greater torque at low RPM. So when we really want to remove metal quickly, these are the typical choice of the 5-axis machine you're going to use.

OK, then we've got a head table machine. So with this machine, we've still got the capacity for using heavy parts because the table isn't doing the tilting. The head's doing the tilting, so all the weight is pointing down the base of the machine directly down. We are getting rotation on there, but these machines are good for heavy parts and reasonably large parts. Again, we haven't got the upstands of the Trunnion, so this gives us, typically, a slightly bigger working envelope, especially in three axes.

Any machines with the tilt on the head-- during 5-axis machining, one of the common problems that we have is exceeding the linear axis, so we may have 1 meter x travel. But if we're tilting the head, then the rotation point is moving beyond, so the actual linear range at the tool tip is often less in 3- and 5--axis machining. So that's another benefit really of the table-table machine, where you get full use of x and y on the part. These machines are often used to put something like a tombstone fixture on so that we can use it, essentially, as a horizontal mill. We get the benefit of chip evacuation using it as a horizontal, and we can quite easily machine parts on four sides of a tombstone.

And then the head-head machines, the major benefit of this type of machine is they are great for large, heavy parts. OK? All of the rotation is made on the head. So PowerMILL, traditionally, one of its biggest markets is automotive mold-making, so there's going to be some large cavity parts on those machines. And generally speaking, they're all cut either on 3-axis or on head-head machines to get the actual size and weight onto a 5-axis machine.

OK, what they're not so good at is heavy metal cutting. So on many of these machines, the motor for the spindle is mounted on the head. Other machines are similar-- and again, I think most of you were in Mike's session. Other machines have a [? mutating ?] head, where we've got it at 45 degrees, and these offer the benefit, for a head-to-head machine, typically, of placing the motor into the machine, and we're driving the spindle with gears. So this gives us, typically, more rigidity and more torque for a head-head machine, but they're not going to beat a table-table machine for heavy metal cutting.

Another problem with these machines-- and if you walk around an automotive mold make who are using them, you will find that they are predominantly doing 3 plus 2 axis machining, or positional 5-axis. I'm not sure what term is most familiar here. And that's because these machines typically have a restriction in the c-axis, so they can't spin around forever.

They've typically got something. It might be minus 360 plus 360. And when you are doing simultaneous machining, which is more than a simple profile, you're likely to exceed that limit. And when you exceed that limit, we have what we call a retract and reconfigure, where the tool has got to retract, unwind, and re-engage. And therefore, we're going to get a lot of entry and exit marks on the part, so they're not typically used for a lot of simultaneous work, but they are capable,

OK, we've got other machines, which I'm not going to talk about here-- turn/mill machines, mill/turn machines, et cetera. Something that we've been quite heavily involved in is robots. So a robot isn't a 5-axis machine. It's a 6- to x-axis.

We support 18 simultaneous axes in PowerMILL. That's six on the robot and 12 external axes. I've never actually met anybody that wants more than that, but, essentially, you can have your robot, which is 6-axis. You can put that on a track on the floor to give you a linear axis. You can hang it from the ceiling in a linear axis.

You can place a Trunnion table on the side to give two additional rotary axes. So some of our customers have done lots of weird and wonderful configurations with robots, which enables them to have a huge working envelope for really quite a cheap machine. The major negatives with robots is their inability to cut hard material and their lack of accuracy.

So you're not going to be chasing microns with a robot. In fact, when the robot arm is fully extended, you might be trying to chase some millimeters. So they're generally used for soft materials where high accuracy is not a requirement. So we will often-- a lot of our customers, they're using them for milling resin or foam of theme park caricatures, cartoon people, and all kinds of art work, things like that. So if you want high accuracy, rigidity don't use a robot. If you want a huge working envelope for a relatively cheap price where accuracy is not important, then a robot is a very viable option.

A lot of CAM softwares drive robots. You know, you create the tool path in exactly the same way. No different, really, to a generic milling tool path. And you'll find a whole host of CAM solutions can drive a robot, but to drive one effectively, you can not use generic milling simulation and post-processing.

So one of the big differences between a robot and a milling machine-- a 5-axis milling machine, when it's not vertical, when it's tilted, there are two solutions. OK? a or b is positive or negative, and c will spin 180 degrees. There's just two solutions. A robot has eight general configurations, where the tool axis is the same on every one of those images. OK, the tool is at the same point, and the tool axis is the same, but the robot is in eight different configurations.

If you look at the last two axes of the robot, it's essentially a very similar configuration to a head-head machine. You know, we've got the pendulum axis at the end, e, and then we've got a rotary, d. Now, to drive these really effectively, we need to be able to determine exactly which of the eight solutions we want because there is pretty much always a necessity to avoid collisions with your part and the robot, and we may have to specify which one of those allows us to avoid collisions.

And other controls which are not typical for a milling machine is prioritizing which axes to use. When we use the base axes, these ones, they're heavy, and they're not so quick, not agile. So we will often-- within PowerMILL, we can add priorities to axes, and we will normally give priority to the more agile axis and use the heavy axis as a second priority. So these are different controls which you really do need if you want to program robots effectively.

The other big problem with robots is the singularity. A milling machine has a singularity, typically the z-axis, but a milling machine, typically, copes with it quite well. We're going to look later at some of the problems of the singularity on a milling machine.

What a robot will do-- a singularity is when two axes are aligned. So any two axes on that robot, if they're aligned in the same direction, that robot will stop. It will simply stop and say, I don't know what to do. So within your tool path, you can't hit a singularity. OK?

But because you've got eight configurations-- and actually, there's more solutions than eight. There's infinite solutions really because we can touch that axis around and compensate for it here. So we have controls to avoid singularities so that they do not occur, and that's very important if you are robot machining.

Some people drive robots from a CAM software which is not really suitable, and they simply pass the robot x, y, z, i, j, k vectors, and the robot software will do its thing. The problem with that is there is no collision control. You hope and pray that nothing hits, and then you hope and pray that you don't hit a singularity. So if any of those things occur, you've got a problem.

So coming back to generic 5-axis. Is it for you? There's some general beliefs that 5-axis is for the super advanced guys, people doing aerospace, blade finishing, or blisk finishing in this case, turbine blades maybe. And you are quite right. It's a very efficient method of manufacturing those shapes.

Others believe it's, you know-- OK, if I do big mold and die, then I need 5 axes. Drilling at different axes is a good example. You know? Instead of lots of multiple setups, we can do it in one or two setups.

Or military and defense, another industry which commonly invests in 5-axis, but the reality is is job shops are buying 5-axis all over the world, not particularly super advanced machining. They're simply buying them because they offer really good efficiency gains. Simple [? parts-- ?] this part on the screen, this part, all have features on them-- I mean, that part is super, super simple at the top, but it's got a few angled walls.

If I've got a 3-axis machine, I'm going to use a ball nose probably, or maybe a form tool, to take those out. Using a ball nose is going to take quite a long time, and I'm going to have cusp all of the way down the wall. Using a form tool is extra cost in tooling.

I could use a standard tool, and tilt the tool, and cut those walls in a single pass, assuming the cutter was strong enough to do so. Similarly for the part on the bottom right, I've got a number of holes on different angles. Let's just drill them all in a single setup.

The part bottom left, I've got some steep walls in an open pocket. To cut those three axes, I need an extraordinary length tool, which is going to invoke chatter, vibration, cause a reduced surface finish. If I can tilt the tool, I can use a much shorter tool-- more rigid, less vibration.

OK, so we've bought our 5-axis machine. What is really common-- I've been in many facilities where they've bought their first 5-axis machine. I go visit them, and they want to see everything moving. You know, they start, and everything is simultaneous.

That's probably not the right thing to do. When we look at multi-axis machines being used by industry professionals, most of the time they are doing 3- plus 2-axis machining. OK, so they'll tilt the tool, use one or two rotaries to tilt, and then those rotaries will be fixed during the milling process. That's really quite common.

3 plus 2 is simple to program. Certainly, for the Fusion users in the room, I'm guessing you do it quite regularly if you have a 5-axis machine tool-- simple to program, very predictable motion. We're going to look at how unpredictable 5-axis can be soon. And a predictable surface finish-- essentially, it's 3-axis machining from a different axis.

3 plus 2 is often faster than simultaneous also. Dependent upon the simultaneous tool path that we're talking about, we can get big swings in the c-axis-- we're going to see some of that later too-- over a very short distance. And quite commonly, the c-axis is the slowest axis on a machine tool.

We've got x, y, z, a or b, and c, and c is the laggard, the slow one, typically. And if over the space of half a millimeter you need a 180 degree swing in c, then essentially that tool is going to dwell there for some time because the c can't move fast enough. So when you've got a lot of this rotary axis motion, you may program your part at 5 meters per minute. It's unlikely to achieve anything like that. OK, a machine can only move as fast as its slowest axis.

And as I explained a little with the head-head machines, a lot of 5-axis machines, some of them simply do not support 5-axis. A lot of the mold makers actually by 3- plus 2--axis machines. They're cheaper, more rigid, and they do the job that they need. It does the job that they need.

And those machines typically have a limited c-axis. I've already explained, plus 360, minus 360. So for a lot of simultaneous work, they're not very suitable.

Now, also in 3- plus 2-axis, the rotaries can be clamped, making them much more rigid, whereas in a generic 5-axis tool path, they're not clamped. They're using an electronic brake Michael? Yes? Good-- which is not so rigid, and heavy cutting can move that, so you're losing accuracy at times when heavy cutting in simultaneous-- more rigidity in 3 plus 2.

OK, so let's have a look at some of the areas where 3 plus 2 obviously beats 3-axis. So here we've got a part, and in 3 plus 2, to machine this part is quite simple. Just use a simple setup, number one, in this vise, and cut the bottom face of the part.

So face it; put in the holes; use them to mount on to the simple fixture, a reusable fixture for other similar parts, potentially; and then do the other five phases in 3 plus 2. Even if there's angled holes, we can cut them all in 3 plus 2 in two simple setups without any expensive fixtures required.

So in 3-axis machining, is really the fixturing and the setting up which is really going to cost you money. 3 plus 2 removes most of that cost.

When we think about precision in 3-axis, every time you take the part off the machine, reorientate it, put it onto a fixture, we're losing precision here, there, and everywhere. Where tool paths should blend beautifully, we start to get some mismatches. This is occurring on-- you know, it doesn't matter how careful you are.

The professionals who really take their time to measure the tool length, they're getting some problems of mismatches. 3 plus 2 machining removes most of that inaccuracy, and whichever axis we're moving down, we all hit the center of the target. Tool paths are matching up much more beautifully.

Minimize tool changes-- this simple part on the screen, we're machining it in 3 plus 2 axis. We're saving time on tool changes. So if we're using the same tool in different axes, then we can essentially order our milling to optimize for tool changes.

In this case, we've reduced tool changes from 11 for 3-axis machining down to four tool changes in 3- plus 2-axis machining. And shorter tools-- so that part that we saw on the screen, if I was to try to machine that in 3-axis, I've got a tool length of 1.4 inches. In 3-axis, I've reduced it to 0.75, almost half of the tool length. Going to explain a little what kind of difference that can make in a moment.

This one-- I was thinking of removing this slide, actually. I don't like it an awful lot, but avoiding the purchase of form tools. So in 3-axis, that angled wall requires a form tool to match the angle, which may not be a standard tool in 3- plus 2-axis. This benefit becomes much greater in 5-axis.

But in 3- plus 2-axis, we could just tilt the tool. If that's a simple wall, then we can cut it all using a standard tool tilted. So again, just to reiterate, what is 3- plus 2-axis? So you're seeing a multiple 3- plus 2-axis tool paths being simulated here.

All we're saying is that during the cut the a or b and c are static. OK? So a, b, c static-- they're not moving whilst that tool is cutting. The transition between tool paths we have motion, but during the cut, they are static. The rotaries can be clamped, given extra rigidity. The code, as Mike explained, can be much more simplified just using [? plane ?] spatial, things like that, and it's very, very predictable results.

So let's move on to simultaneous 5--axis. OK, so this is where we are rotating the one or both of the rotaries during the cut. OK, it requires more thought on programming. It's more complex, and we have much more complex, less predictable machine motion. Again, I'm going to look at this in a bit more detail as we move along.

And here is an example of simultaneous 5-axis machining. We can see in this case, both rotaries are moving, which enables us to use a very short tool to machine the base of that open pocket.

OK, some of the advantages-- let's just think about the contact point of the tool. Any machinist here will know quite well that a ball nose tool doesn't cut well on the tip. If we've got indexable inserts in the tool, then this 4-flute tool, at the very tip, you actually only have two flutes, and therefore we've reduced the number of teeth that are engaged in the cut. Where tilting it, we've still got four flutes and a larger effective diameter.

I just basically stole this data sheet off the [? Sandvik ?] website, so you can go on this if you want. It's just on the [? Sandvik ?] site, and you'll see here they give us parameters for a non-tilted cutter and parameters for a tilted cut only at 10 degrees, 10 degrees away from the surface. Now, the important thing to look at is the feed rate.

If you're not 2.8 meters per minute, if we tilt by 10 degrees, 5.1 meters per minute. So we've almost doubled the feed by applying that 10 degree tilt. That's really quite dramatically reducing the cycle time of the part.

For super finishing, basically they've said, you can't use a non-tilted cutter. You can't use one, and we're going to give values for that. And then we have the values if you are tilted.

So here is a couple of examples. So the first tool path is OK in most places. In most places it's OK, but there are points on that tool path where you are not tilted, and therefore, the surface finish will not be so good. And what people generally do is reduce the feed rate for the whole tool path to compensate for the areas where it's not cutting well. Whereas on the right, we've always got the 10 degree tilt measured from the normal of the surface, and therefore, the cutting conditions are really very consistent, which enables us to use optimized feed rates to cut that part.

So this is another area where simultaneous machining is used greatly, where we're using the form of the tool. In this case, we've got a conical ball nose tool, and we're using the side flutes of that to cut that aerospace component. The reason we're using that particular tool is the part is in an undercut situation. We would have to put that in a fixture for 3-axis machining.

If we wanted to 3- plus 2-axis machine that part, we're probably going to have to just use a generic ball nose tool, in which case we're going to have to do a lot of passes to get an acceptable surface finish. But using the sidewall of this conical tool, we can take as large as steps as the tool can take. If the tool could handle a single pass at the bottom-- well, it's not tall enough. Maybe it could do it in two passes and cut that whole sidewall.

We've used a conical tool because there's a small fillet in the bottom of that part, and we don't want to use a generic ball nose because it doesn't have the rigidity. So using conical tools for things like that adds rigidity, enables us to cut the fillet in the bottom. And of course, I have the benefit of a very large step, which reduces cycle time.

Here's another example where we're using really the geometry of the tool to improve finishing-- improve both the surface quality and the cycle time. So here we're using just a pretty standard tipped-radius flat-bottom tool, but we are really just applying a lead angle to cut on the leading edge of that tool, which is always measured from the normal of that blade. There's a few subtle things here which PowerMILL does, which you can't really see. One of the problems of cutting blades like this on 5-axis milling machines is, as the tool passes the leading or trailing edges of the blade, then the acceleration goes crazy, and we start to lose accuracy on many machines when we push the acceleration to the max. They don't hold their tolerances so well.

So what PowerMILL will do in instances like this, and it's not overly obvious, but it can start the tilt before and finish after the leading and trailing edge, which is just dampening the motion of that rotary. So subtle controls like that become important on parts like this because having quality on the leading and trailing edges of a blade is very important.

We looked at swarf machining with the conical tool. A lot of people actually use swarf machining or try to use it. You see a surface on your part. It's got straight edges, and we think, [? now ?] we can swarf machine that. It's a common thought, but most of these shapes are actually not possible to swarf machine them.

A definition of a swarfable surface is a surface which can be unwrapped, a developable surface. So a cone is perfectly swarfable, no problem. You could unwrap it in a piece of sheet metal with no stretching, no compression, perfect, assuming zero thickness. So a pocket with angled walls and fillets in the corner, you could unwrap that. It's perfectly swarfable.

But many shapes on parts that you receive, they look like they're swarfable, but they're not because they're not unwrappable. And so any piece of CAM software-- PowerMILL, Fusion, and all of the others-- they will try to apply approximations because it's not possible to swarf them, but users want to swarf them. So essentially, we do apply approximations. PowerMILL always has a rule.

We will always leave metal on, not take extra off, but you can't machine those things properly with a swarf tool-- which is why a lot of customers are now buying barrel tools, which give many of the benefits of straight-sided swarf cutting because you have a very large convex radius on the sides of a barrel tool. Gives us many of the benefits, but you don't need a perfectly swarfable surface, OK? So that's some of the major benefits that people use with barrel tool machining.

OK, this video, which I rudely spoke over, is really showing, again, cutting the base of that open pocket, which is not flat, and the walls are in an undercut situation. So compared to 3-axis so a 3 plus 2, we're not going to be able to machine all of that base with either of those strategies. If it's 3-axis, impossible. If it's 3 plus 2, you're not going to machine [? it ?] [? all. ?]

This is a [? 3 ?] plus 2-axis tool path. The user, which was me, took great care to choose the best axis I could to hit that base surface. But unfortunately, some of it was still shielded by the side wall, so this area on the right-- I don't know whether you can see, but there's an edge down that base which I simply can't machine in 3 plus 2. So I'd have to choose a another tool path, two 3- plus 2-axis tool paths to get it all, and then I've got transition marks between them. In 5-axis, I can hit it all in a single tool path, no transition marks, a much nicer result.

OK, reduced stick-out length. Now, to get my optimum axis in 3 plus 2, there is some rotation on that, but to get as much of that base as possible, my axis was close-ish to vertical. And as you can see, the tool length was ridiculously long, so I'm going to have to tread very, very gently with a tool of that length, cut it very slowly, I can't really apply much force on the tool at all. Otherwise, it will break.

Moving into 5-axis, no problem at all-- a nice, short, rigid tool assembly. OK, so in this case we reduced the to length from 3 inches to 1.5 inches. Here's just a graphic of 3-axis. Tool length is not too bad on here, but if I've got excessive stick out, what are the problems?

The biggest problem is greater tool deflection. So especially when we're cutting on the side, we're getting massive deflection on the tool, which, of course, produces poor tolerances. It increases the probability of chatter. Chatter is a complex beast, but when you have longer and longer tools, you're increasing the probability of it occurring, which is going to give you poor surface finish, reduced tool life.

As that thing is vibrating, it's damaging the edges of the tool, and once that goes to a certain degree, then catastrophic failure normally soon occurs. Just something I got off the CNCcookbook.com, which I would recommend anybody reading if they haven't done so. But just a simple stat-- rigidity increases as the third power of stick out.

So if we reduce the stick out from 1.25 to 0.75-- so we haven't halved it, but we're moving along that way-- it buys us 4.63 times more rigidity. So a lot of our good customers, they're not, especially in challenging situations, using standard length tools for all of their jobs. They are actually checking with PowerMILL-- what is the shortest tool I can possibly use? And then they're setting their tools up for the job with the shortest length tools because it makes such a big difference to the final accuracy and surface finish.

OK, here's three different ways to use your 5-axis machine tool. So we could machine that part. It's quite a simple part. I'm going to show you a bit of this live.

The first option is 3- plus 2-axis, where we're having to do it as two separate tool paths, essentially. So there's no simultaneous motion there. The big problem there really is I'm going to get transition marks on the top of the part, where we've entered and exited on each part, so it's going to need additional polishing in this instance.

But if we had a complex feature-rich part, lots of pockets, bosses, and all this kind of stuff, then it's really-- the big problem here is the programming time is enormous. Just I'm going to set up a tool axis here, cut that piece, set up a tool axis here, cut that piece. Programming time is really big. We end up with a patchwork quilt of too paths with transition marks everywhere, which is going to increase the polishing necessity.

So in this instance, we've machined it 4-axis, where we're only using one of the rotaries, and a big benefit of that is, especially on head-head machines, I'm not going to hit the restricted c-axis limits. I'm just fixing the c-axis, and I'm going to use the a or b axis to cut that part. No problem with the retract and reconfigure, and it allows me to cut that part without any problems. Also, the speed of the c-axis-- we've already spoken about that. The slowest axis typically not a problem here because we're fixing the c-axis.

And the final option, which is simultaneous 5-axis, the real benefit of that is, especially on more feature-rich complex parts, it allows us to use the shortest possible tool of the three instances. I'm just going to pop to PowerMILL just for a moment just to show a little bit of this. So I've put a tool path on that part. It's what you guys, most of view-- is there any PowerMILL people here? Ah, there is a few.

So in PowerMILL we call it raster. In this case, it's an optimized raster because there's some steep walls going in the wrong direction, which a raster tool path wouldn't do a great job of, so in PowerMILL we have an option to optimize it, but that's not my point in this case anyway. This tool path is 3-axis, and I'm going to need quite a long tool to avoid collision-- not too bad in this case, but still, that's kind of the worst place on the part. And if I just press Play, there we go.

So we've had to use that length of tool to avoid any collision. PowerMILL will tell me what the minimum tool length required is, and that's pretty much what I've used with a specified clearance. With 3- plus 2-axis machining-- again, this is something all of you do, I assume. I can cut half of it in 3 plus 2 and then cut the other half in 3 plus 2, so nothing to get too excited about there, but the problem is I'm going to have transition marks on the top.

OK, 4-axis, this is what I would probably use on a head-head machine for a part like this because, again, I've got no problem by hitting retract and reconfigure on the head. OK? I'm not spinning the c at all.

And then, I've got a 5-axis tool path. Let me just start that one and press Play, and there we can see this gives us the possibility of using the shortest possible tool. Now, the c is all within range of the machine. This is a restricted c-axis machine, but this tool path is all within range, so it's all going to be OK.

And there you can see-- so in PowerMILL, we call this automatic collision avoidance. Its primary objective is to avoid the collisions, but it has other important aspects to it. Do not give us any sharp, jittery, high-acceleration rotary moves. Anticipate [INAUDIBLE] well before you hit it, and start a nice, gentle rotation in advance. So that's really the nature of the function in PowerMILL.

But we also use it, what I say, to make steep areas shallow. So typically when you've got a part with steep and shallow areas, typically in PowerMILL, we would, say, use raster or 3D offset and constant z. In Fusion, I'll translate that. That's contour for the steep and parallel or-- what's the offset one called again? Scallop, thank you.

OK, and that's typical because people don't want their tool to meet up to a steep wall and go up it because it's likely to break the tool. Also, they don't want it to go along here and go almost vertically down because the tool doesn't react very well to that. You were getting push off, chatter, vibration. It doesn't work so well.

So what we'll often do is use a more simplified strategy like parallel raster but tell PowerMILL, really, to-- I give it, essentially, a greater clearance distance from the head. And it's what we call-- what I call-- "it makes steep areas shallow." That tool is-- when you look at the inclination of the tool to the underlying surface, it's not a steep surface anymore, not particularly steep. So it allows us to use a more simplified strategy on complex parts without worrying, is the underlying surface steep or shallow? Because this makes everything reasonably shallow, depending upon the settings that we give it.

OK, so another common problem here. We've got very, very simple facing operation. I've go 10 minutes left, so I better be quite quick. On a [INAUDIBLE] machine, no problem at all. That part fits on that [INAUDIBLE] machine beautifully. Now, a lot of the big shops I visit, one of the things that they want for scheduling is, "I want to put my part on the smallest possible machine."

You know, they've got 40 machines all running. They don't want to put a small part on a big machine. You've just lost the capability of that big machine. So here we've put this part on a smaller machine, a Haas machine.

And unfortunately, as we can see-- I don't know whether you saw that. Let me play it again. I'll just go from here-ish. What we've done is we've exceeded the y-axis limits of that machine.

Now, PowerMILL will tell us, can we move the part a little to get it within limits. It will give us the range, depending upon what tool paths are in the [? MT ?] program. It will give us the min, max x and y range to allow us to move the parts if necessary. Here it's telling us, "I can't do it. I've exceeded the limits of the machine."

So instead of moving the part, which is time consuming, we're just going to reprogram this slightly differently-- same tool path, still essentially 3-axis. Let me just move on-- 3-axis, but what I'm going to do is instruct PowerMILL to replace the y motion with c motion. So now I've got the y absolutely static. It's all fixed on 0, and I'm replacing it with c. Now, everything's within limits, no problem at.

Here's another very common problem. This was a machine tool we had, not anymore, in our-- we've got an inbuilt tool room in our offices in Birmingham. This was on a Huron Control Siemens 840D programmed at 7.5 meters a minute. It's not running even close to that.

And if you look at the c towards the end, it goes really quite jerky-- duh, duh, duh. We've got the high-speed cycle switched on on the 840D, and that's kind of the best that we got. So what's the problem with that jerky motion? Two big problems-- one, time, cycle time. It's not running close to 7.5 meters a minute, which is what that tool is capable of. Probably a worse problem is every time you get a dwell on the part, we get a mark on the part.

So imagine smooth cutting. Your tool is pretty much always deflecting, but it's consistent because we're moving quite nicely. So we're always leaving a little piece of metal on. If it's within tolerance, it's cool.

Once we stop for a moment, we allow that tool to relax, and it just-- it's actually the most accurate part of the job, and it looks like a gouge, and it's going to require a lot of hand-finishing. So we don't want that. So how do we avoid that?

We change the way we put points on the tool path to suit the control. So for most tool paths, you put enough points in to adhere to your tolerance that you require. So if it was flat, you'd put a point on either end. You don't need any intermediate ones. If it's gently curving, the points of spaced quite far apart. For high-curvature parts, we need more and more points to attain the tolerance.

So the tool path on the right has got far too many points that we need, far too many. This is what we call redistributed point data, where we supply a maximum distance of points. And I put a maximum distance bet-- typically, will be something like 0.3 millimeters, so you get really dense points on your tool path. But the results on many common controls-- this is the same tool path, essentially, running at the same feed rate.

One's got enough points, and this one's got far too many points to hold tolerance. The second one runs very close to the programmed feed rate-- the first one, nowhere near. The cycle time is 39% saved by adding all of those extra points. Most importantly, the surface finish on the second one is really beautiful, and on the first one, a lot of hand-polishing is required.

So the way we put points on the tool path needs to be really specific to the control. My experience-- [? Haydn ?] [? Haynes, ?] we can really put lots and lots of points. They love points, and they move just beautiful. Siemens, the block time calculation is not so quick, so we space them a little bit further apart, so it needs a little bit of trial and error.

OK, here we're cutting the most simple part ever, a sphere. I'm just going to pop into PowerMILL for a moment. So I'm going to cut a sphere for you normal to the surface. So the tool like this is always pointing towards the center line at the center point of the sphere, so very, very simple.

And I'm projecting two lines onto the part, one exactly through the center point, the apex of the sphere, and the other one 0.1 millimeters away. So one's above the center. The other one moved 0.1 millimeter on a 200 millimeter diameter sphere, so very, very simple tool path.

So the first one is at Y0. So let me just simulate from the start and press play. So it's normal to the surface, but I've added limits so that it doesn't go beyond 45 degrees. OK? Otherwise, I have the potential of hitting the holder.

OK, so it looks nice. Everybody agree? Anybody think it doesn't look nice?

AUDIENCE: The top center hits the center point of the tool.

CRAIG CHESTER: Agreed, agreed. So we could have applied a bit of lead. No, we could have applied a bit of lead. Actually, at the top center it's more than the top center. Nearly everywhere is on the tip of the tool, apart from where it's limited.

AUDIENCE: Oh, that's true.

CRAIG CHESTER: Yeah, so you're right. That's a problem. We could have applied some lead to overcome that. Generally, though, it looks OK, aside from that. It's a very good point.

Let's have a look at this one. This is the one where the lines moved 0.2. Could have made it 0.1-- I just wanted it to make it enough so you could see it.

So that one looks as good, right? Looks as good. Anybody disagree? I think it looks as good. No real difference-- I can't see a difference.

OK, let's go back to the first one, and I'm going to switch on the machine tool that it's going on. OK, let's simulate from the start, and there we go. Nice, looks nice to me. I like it.

Let's have a look at the second one. Anybody see something bad happen? Just keep your eye on the head of the machine tool at the top-- boom, spin 180. And that is going to damage the part. So that is not very nice behavior.

So why is that? Well, that is the very nature, the kinematics of that machine tool. That's what it does. If you want to point to the center of the sphere, that's what that machine does, and most 5-axis machines-- head-table, table-table-- they're all going to have a similar problem. That's what will happen.

So the problem is that rapid rotary axis acceleration, it typically occurs when the tool axis is in simultaneous motion, never, of course, in 3 plus 2. Since simultaneous motion close to what we call the singularity of the machine-- the singularity of nearly all 5-axis milling machines is 0. And when you've got simultaneous motion very close to 0, that's when the c-axis becomes unstable, as we can see in this instance.