Augmenting Manufacturing with Machining Dynamics

MICHAEL GOMEZ: Good afternoon. My name is Dr. Michael Gomez. I'm a principal R&D engineer here at MSC, and I lead our manufacturing research and technology team. And today, I'm here with Dr. Tony Schmitz. Tony.

TONY SCHMITZ: I am Dr. Tony Schmitz. I'm a professor at the University of Tennessee, Knoxville, and consultant with MSC.

MICHAEL GOMEZ: And today, we're really excited to show you something we've been working on titled augmenting manufacturing with machining dynamics. First, we'll go through our safe harbor statement. Of course, the presentations during this event may contain forward-looking statements about our outlook, future results and related assumptions, total addressable markets, acquisitions, products and product capabilities, and strategies.

Man, I messed up. I'm sorry. I shouldn't even read through that.

All right, I'm going to-- let's just restart from the top. My bad. All right, 3, 2, 1.

Good afternoon. My name is Dr. Michael Gomez. I'm a principal engineer at MSC Industrial Supply Company, leading our manufacturing research and technology team. And I'm joined today with Dr. Tony Schmitz. Tony.

TONY SCHMITZ: Hi, I'm Dr. Tony Schmitz. I'm a professor at the University of Tennessee, Knoxville and consultant with MSC.

MICHAEL GOMEZ: Today, we're going to be talking to you a little bit about something we've been working on, which is augmenting manufacturing with machining dynamics. We have our safe harbor statement. And then now I'll pass it over to Tony.

TONY SCHMITZ: Thanks, Michael. We have three primary learning objectives for today's presentation. The first thing we want to do is apply machining dynamics principles through some advanced simulation tools, and we'll show you demonstrations of that. The second thing is we want to integrate MSC's machining dynamics add-in that we've recently developed within Fusion's manufacturing workflow. And then finally, we want to use this information to discover the productivity and operational efficiency improvements available to us, to us through the selection of optimal tool and process parameters.

So let's begin by looking at part production workflow and manufacturing environments. We're specifically interested in the red zone. We begin with design analysis, but then in this red zone, we call this the pre-production planning phase that leads us to production, machining, post-machine finishing, and then our quality control. So let's take a closer look at that red zone, this pre-production planning phase.

Our key activities include selecting the materials for the workpieces that we're going to produce, determining the machining processes, which lead us to our desired outcome, and then planning the order of those operations. We use CAM software in order to program the CNC machines and develop the toolpaths that are required to machine our parts. We then have to set up the machine tool for those operations. This includes selecting tools, the right fixtures, and then the tool offsets based on those fixtures and the cutting tools we've selected.

And then finally, we want to check and see those results before we move into the production machining sequence. So that sounds great. What can go wrong?

If we look at those individual elements, here are some things that we have to pay attention to. We're selecting machining processes, but it might be that we haven't selected those machining processes in an optimal way. So we might want to revisit the design specifications and adjust our plan based on the materials for the workpiece, the cutting tools, and the machining strategies.

Second, we can have toolpaths or cutting parameters that are embedded within those toolpaths which are incorrect. We can use simulations to reveal if we've had tool collisions, which would be an unexpected and undesired outcome. But we can also have inefficient toolpaths that have cutting parameters, for example, that lead to poor surface finish or accelerated tool wear.

In this case, our feedback loop includes reviewing those toolpaths, our tool choices that go into generating those toolpaths, and then the cutting parameters that are inherently included in those toolpaths. Next, we have to set the tool offsets and set up our machine tool. And we can have misalignments in that process as well. So we have to pay attention to our setup and our tool offsets.

So our feedback, in this case, can include what tooling did we select? Is the fixture appropriately arranged? Are we clamping the part correctly? And then whatever offsets may be required within the part program, are those completed correctly before we execute that part program? All of these combined lead to the outcome to prepare us to produce that first part.

It turns out all those errors that may have happened before can compound, and they're kind of hard to unravel once we get to that first part. And so our interest here is in trying to make the best decisions that we can at this pre-process planning stage in order to minimize the amount of trial and error and feedback and repetition that might be required to get us to a production sequence.

All of that points to cost. So we know manufacturing costs can be divided into several categories. So we see here a graphic from Sandvik that divides those manufacturing costs into cutting tools, our buildings and administration, the labor, machinery, and finally, the workpiece material.

What we see is the cutting tool cost actually makes up a fairly small percentage of that total cost, but this can be misleading because the selection of the cutting tools leads us to selection of our cutting parameters. And those cutting parameters have everything to do with cycle time. If we can reduce the cycle time by increasing our cutting speed, that leads to added capacity for our shop floor.

When I increase capacity, the relative share of these other components decreases over a full production cycle. And so I can have tremendous cost savings if I can make good decisions about how I use my cutting tools at this pre-process planning stage.

So how do I get to those process parameters today? One way is by relying on my expert machinist and programmers that I already employ. They will base their decisions on past experience, so they have insights which they've gained over several years of machining, this part and similar parts.

Trial and error is another approach that we can sometimes use. We have to modify parameters based on the process outcome. Did we get the right surface finish? Is our part accurate and meet design tolerances? And then finally, if it's a process that I haven't spent a lot of time thinking about previously, I may have to make my best guess and then use manual intervention as the process unfolds.

My second big resource for selecting process parameters is the tool supplier. So there are cutting catalogs that might be physical catalogs or probably more likely online. And so I can use those to select my spindle speed, feed per tooth, depth of cut based on the tool material, the geometry of that cutting tool, and the work material.

There are also interactive tools and calculators that I can leverage, which are available online where I enter details about my cutting process, such as the work material and the tool diameter, and then I receive recommended process parameters from that calculator. And finally, the CAM software that I use probably has built in tool libraries that are going to include recommendations for how to use the tools, which are contained within those libraries.

So everything's good. But do we have the full picture? Let's see what else we might want to consider.

The big outcome that we'd like you to take away from this presentation is that machining is more than geometry. Along the top ribbon, I see the digital representation of machining parts, so I begin with CAD, where I have my part design. I have to select my cutting tools that are going to remove material to reveal that design from my preform. And then within the CAM software, I can generate toolpaths.

Once I have those toolpaths, I can then simulate those toolpaths to confirm that the tool moved through space in the desired trajectories to remove material and reveal the part that I want. But there's more. Now let's look at the bottom ribbon and see how that affects how we'll make decisions about cutting parameters.

The first is a measurement that we can use that we call tap testing. That allows me to identify the structural dynamics. This is how a system wants to vibrate once I've put it together. If I have those structural dynamics, I can generate a map.

So that map is shown here. It's called a stability map, and it lets us select machining parameters at this pre-process planning stage.

Once I've selected that point, I can then use simulation to say what's the force and vibration that's going to occur during that machining operation without needing to actually execute the machining operation to see what's going to happen? That's the value of simulation. So let's talk a bit more about this tap testing process.

So in the picture, we see a schematic with a hammer and then a wire attached to the tool, which has a tiny accelerometer attached to it. So this hammer allows us to input a known force into our tool holder spindle machine system. The accelerometer measures the vibration in response to that force.

If I have those two signals, then I can generate something called the frequency response function. So this describes our structural dynamics. It says, how does my tool holder spindle machine want to vibrate when the cutting force acts upon it? That frequency response function captures information about natural frequencies, stiffnesses, and damping values that describe how my system responds to force in the form of vibration.

If I have that information and a cutting force model, I can generate my stability map. So that map is shown here as the third picture. The vertical axis is my axial depth of cut or my step down in my CAM software. The horizontal axis is my spindle speed.

Between those two, now I have information that lets me select cutting conditions that will lead to stable operating parameters. The thing we're trying to avoid is chatter, a self-excited vibration that has large forces, large vibrations, and poor surface finish.

The blue line in that map is the one that separates those two conditions. Above the blue line is where we would expect to see chatter from combinations of axial depth and spindle speed. Below the blue line is where we'd expect stable cutting conditions. Again, combinations of axial depth and spindle speed that will let me get the desired outcome.

So if I have that map at the point that I'm selecting my process parameters in this pre-processed planning stage, I can make good decisions about those combinations that go into my CAM software. Once I select a point, represented here by the blue dot, now I can simulate to say, what will the force profile look like? What will the vibration look like because that's going to influence the quality of my product?

The outcome of all of these steps is that I can reduce this trial-and-error approach, which is often necessary for us to select successful cutting parameters. So this notion of machining dynamics gives us a new toolbox that we can carry with us into this pre-process planning stage.

I talked about modal tap testing. You can see a photo here. So there's a gentleman with a modal hammer that's tapping a tool, which is mounted in a spindle. And a machine tool, the accelerometer, is attached on the opposite side.

So I collect those signals. And in software, I'm able to generate that frequency response function and then select machining conditions that are either stable or produce chatter, which is that bad surface finish that I don't want.

Now, there's an important thing for us to consider here, and that is each time I change my tool or holder or spindle, I change that vibration response. So if for example, I have a tool inserted in a collet holder and I've measured that combination, but then the tool wears out, and I put the tool back in.

If I don't use the same stick out link, my vibration response can change. Or if I have the same cutting tool and the same stick out length, but I change the holder. Maybe I went from a collet holder to a shrink fit holder, again, that vibration response can change.

And finally, if I take the same tool and holder, but I put it in a different spindle, I may find a change in that vibration response. So that highlights the relevance of this tap test, which lets us know specifically, how does your tool holder, spindle, machine combination want to vibrate? And then we can use that information to select machining parameters.

All of that culminates in this stability map. So we've seen this before. In this case, you see a red zone. That is the combinations of axial depth and spindle speed where we would anticipate chatter. The white zone is where we would expect stable cutting conditions, so that's where we want to select our parameters.

The yellow zone just accommodates the fact that in all models, there is some uncertainty. And so the yellow zone indicates, hey, you're getting to an area where you may have a little more risk in selecting those parameters, but many times, that risk may pay off with reduced cycle time and then cost savings, which go with that.

That diagram, as we mentioned, is specific to a particular toolholder, spindle, machine combination and radial depth of cut. You'll see an example here in a bit how that diagram changes as we change the radial depth of cut. The outcome is that that map depends on what we're machining with. That means that the static handbook values we often rely on may not be representative of your dynamic system. So we want to include dynamics to get that stability map rather than relying on these handbook values which don't know where your tool was placed and what machine you were using to carry out your operations.

So the next thing that we want to talk about is an application of these maps to a production of a part. And I'm going to turn it over to my colleague, Dr. Michael Gomez, to talk about that.

MICHAEL GOMEZ: Awesome. Thank you so much, Tony. So the next phase here is we'll be talking about augmenting Fusion workflows using these stability maps. And the showcase we're going to show you today is this aerospace panel case study. So let's start at the beginning here.

So why did we pick this aerospace panel geometry? Well, there's a few reasons for why we wanted to do this. So the first reason is we want to compare these kind of machining dynamics recommendations from the maps that you heard about from Dr. Schmitz here against supplier recommendations or against these static dynamic handbook values.

So what is the value in moving beyond these generic supplier recommendations and incorporating machining dynamics into everyday operations? Again, what you'll see on the right-hand side is the geometry we chose for this case study. We modeled this after a typical aerospace panel geometry. It's a complex geometry with some thin-walled sections. In this case, we just chose a 6.4 to one thinwall ratio.

Another feature that was really unique to this type of part is that there's a large volume of material to be removed in these intricate pocketed areas, which is pretty indicative of other aerospace types of geometries. So what you see for the part there on the right-hand side, we're showing you the stock volume in both inch and metric values, the part volume, and then, of course, the volume of material that's going to be removed to achieve our final geometry. So in this case, we're removing about 93% of the volume of the material in order to get to that final bracket.

So the first thing that we want to step in through or step through here is our toolpath selection. So everything that you heard about earlier today is really about process parameter selection. We're not necessarily optimizing the tool path specifically. However, with the given tool path, we're optimizing the process parameters that are used to machine that part. So the best way for us to show that to you is to highlight the variety of tools we use to make this part.

First, we're doing a facing operation, followed by an adaptive clearing operation with a 1/2-inch endmill. We then move to a 2D contour with a 3/8 inch endmill for rough and finish operations. And then we do a locating bore and then chamfer mill, that last geometry.

So what you see on the right-hand side is actually the outcome of the Fusion simulation. And then what you see on the bottom right here is what the part actually looks like after that first setup. Following the first set up, we will flip the part over. Again, you saw that locating bar on top. That's what we're going to locate off of to machine the back half of this geometry.

Again, if we look at that tool geometry on the left-hand side with those cutting parameter-- I'm sorry, the toolpath-- I'm sorry-- the tool paths that we selected. So we have adaptive clearing, facing, morphing, adaptive clearing, chamfering and so on. Again, it's going to use that same three inch, 1/2 inch, and 3/8-inch endmills, followed by that 1/8-inch chamfer mill. And then you can see that final geometry start to come into play here.

So again, on the bottom right image is that final finished part. If we look at that Fusion simulation, you can start to see the pockets start to take hold. There's that adaptive clearing operation for both roughing and finishing. And so we'll just let the simulation play so you can see that final geometry.

And so when we take a look at our toolpath selection, what do we notice? We notice that this 1/2-inch tool is responsible for removing the largest volume of material by a significant margin. In this case, it's about 80.4% of that 93% of the volume that we were removing originally.

So what are we going to-- what is our next step here? So we know that optimizing this tool's performance through tap testing can help us achieve the maximum material removal rate without risking chatter.

So if I take a look at that table there on the very bottom of the screen, I can see each tool, and I can see the total volume of material removed. I could absolutely tap every single one of these tools. However, you're going to start to get diminishing returns. So in this case, this is the tool that we're going to focus on. So for our case study, the tool paths were actually kept constant between each case study example, and the 3-inch face mill, the 3/8-inch end mill, and the 8-inch chamfer mill were not optimized due to their limited contribution to the overall material removal.

So the focus of our case study, as I mentioned previously, is really comparing supplier recommendations to our machining dynamics recommendations. So in this case, we selected three tools from three different suppliers. You'll see tool A, tool B, and tool C.

You'll see the details of those tools in the following bullet points. Each one of these tools was 1/2 inch in diameter. Each one had a cutting length, or a flute length, of 1 inch.

There were some tools that were three flutes, some tools that had four flutes. They were all put in shrink fit holders, and they all had a consistent overall length. Now the stick out lengths did vary slightly, and we'll talk about the implication of that later. However, we did select these three different cutting tools to compare these supplier handbook recommendations against this type of machining dynamics strategy.

So earlier, you heard Dr. Schmitz talk about the frequency response function. And so what I have here are images of those three tools. And on the bottom panels, you'll see those frequency response functions that we measured.

OK, here's what's really unique here. You saw the geometries earlier. That says that's the same diameter. They all have the same cutting length. There might be a smaller stick out length.

However, that dynamic response has changed. And that's what I see in that bottom panel. And so at the end of the day, what can I start to think of this as? These are actually unique fingerprints for my machining dynamics strategy. So each one of these fingerprints would represent something different and something unique about this tool holder machine assembly.

Now, what does that manifest itself as? That manifests itself as a stability map. So earlier, you might say, well, I don't really know how to interpret those plots. Well, now we go back to our stability map. Let's keep up with this theme of machining is more than geometry.

Each one of these fingerprints is a unique signature to this tool holder machine combination. And as I look at my stability maps, as we'll take a deeper look later, that has some serious implications as to what type of performance I can extract out of these cutting tools.

And so the next thing I'm going to do here, since this is a technical demonstration, we will actually pull up our Fusion workspace so I can show you what this add-in looks like. So right now, I'm in our Fusion 360 workspace, and you can see this aerospace geometry panel that we had just showed you earlier in the presentation. And what I'm going to do is I'm going to first select a toolpath. So we mentioned that this 1/2-inch tool removes a significant amount of material. So I'm going to select this roughing tool path, which is an adaptive clearing tool path, for these different pockets.

Next, we'll go to our utilities tab. We'll go to add-ins, and then we'll run our MSE machining dynamics add-in. What we're going to see is a few options on this screen.

So the first step is that we want to select a data file. So this data file is effectively the outcome of that modal tap test we talked about earlier. So that data file contains information about the structural dynamics of my toolholder machine combination so that I can use it for process and simulation later.

So we'll first start by selecting a data file. So I'm in a tool A workspace. I'll select my tool A data file, and then I have a few options when it comes to showing information. So the first thing I'm going to do is select plot for all of my dynamics, and I'll show that here on the right-hand screen and we'll pull up that figure one more time.

So this would be my frequency response function. Earlier, Dr. Schmitz mentioned that we're showing information on natural frequencies, stiffness, and damping for the structure that we just measured. What you'll see here are measurements for my cutting tool in both the x and y directions of my machine tool. And you'll also see a line for measurements of our workpiece dynamics.

Sometimes the workpiece dynamics can have a significant influence on the performance of my cutting operation. Think about times you're machining very, very thin-walled parts or very complex geometries. Those workpiece dynamics might become significant, and you might have to consider them later on. As a matter of fact, we can absolutely do that today. But for the purposes of this demonstration, we're going to focus on the tool dynamics.

So I'm going to close out here, and we'll just focus even again on this tool dynamics in the x direction. Again, what you'll see is that each peak that we see here is a natural frequency. Each one of those natural frequencies is going to have a corresponding stiffness and a corresponding damping ratio that describe the dynamics of that system. What you see in the red line there is actually a measurement that we call coherence. That measurement is really indicative of how much energy have I put into the system via tap testing versus how much I'm measuring out with that accelerometer.

We like to use that to help quantify our measurements. So we like to show it just to see that, hey, my coherence should be something close to 100% but no less than maybe 70%. And as long as the coherence is above a certain threshold, I can trust that information that I'm getting from my modal tap test.

The last thing we're going to look at here is a plot of our default stability map. So we talked about stability maps earlier in the presentation. This is actually a stability map at a 25% radial immersion case for my cutting tool. We'll talk a little bit more about what that means specifically and how we can change that. But this is the image you saw on that previous slide.

Again, you have a plot that shows the red zone for unstable cutting zones. You have the white zone, which represents stable cutting zones. And of course, every measurement has some uncertainty, and we incorporate that uncertainty into our model.

Something that's really unique about this add in is because of the Fusion API, we're actually able to pull information from the cutting tool that is really useful for us to use. One of those pieces of information is my maximum cutting depth. So you heard me mention earlier that each one of those cutting tools had a maximum cutting depth of 1 inch, so about 25.4 millimeters, in this case.

I've plotted it over the stability map, and effectively, that's the maximum flute length that our axial depth I'm actually going to be able to achieve with this cutting tool just based off of the geometry. However, what you'll see is the intersection of that line between my stability maps means I won't be able to use that entire flute length all the time. And we'll talk a little bit more about what that could look like and what that means for customers at the end of the presentation.

The second tab I want to show you is our simulation tab. So we talked about process parameter selection. How do I select my process parameters?

So the first challenge is toolpaths, and there are other fantastic tools, much like the built-in tools inside of Fusion, that let you select the proper toolpath to make the geometry you want. However, when it comes to process parameter selection, that becomes a little bit more complicated. And so I selected that toolpath earlier.

And again, with Fusion's open API infrastructure, we're actually able to pull information about my cutting tool description. You see, it's a type-- a tool A definition, a 1/2 inch diameter. It's a flat endmill, three cutting flutes. The cutting length is 25.4 millimeters.

You can see our feed per tooth, spindle speed, radial depths, axial step down, and then cutting direction. I'll point out the axial depth of cut is a unique situation here because a feature-based machining, we're actually only going to be cutting at a maximum depth of whatever that panel height is. However, we can talk about the implication of that a little bit later on.

The next features you'll see on this tab are sliders for both radial immersion and axial engagement. And you can see that as I change this slider, that radial immersion value right below there is also changing. So I can set it to a certain percentage. So maybe we select 30% radial immersion, and I can see what that means for my cutting tool geometry. So in this case, it's about 3.8 millimeters.

The next piece I'll focus on is axial engagement. So in this case, you can select any value. We could select-- let's just assume 50% in this case. So I'm cutting with 50% of the cutting length available to me, which would be about 12.7 millimeters, in this case.

And finally, I can select spindle speed. So what spindle speed would I like to run this at at? What spindle speed would I like to check this at?

The default in this add-in is 8,000, but you can change this to any value. So in this case, we're going to pick 9521. And then what we're going to do is simulate.

I have a nice pop-up that tells me what I'm simulating at. We'll let that simulation run. And while that simulation is running, I'll talk a little bit about what's happening in the background.

What's happening in the background is that we're indexing the stability map that corresponds to that 30% radial immersion value. And so I get the following plot here. That green dot shows me the process parameter points I selected for my cutting operation.

I see that point is green. It says it's a stable cut. How do I know it's stable? Well, let's take a look at our cutting force measure or our cutting force plot and our tool vibration plot.

So if I make this a little bit bigger-- we'll pick a zoom-in tool-- and we'll just look at a section of my resultant cutting force. And then we'll also do the same for our resultant vibration. And so you'll see a few things on this plot here.

So the first is we are showing you an actual time domain simulation of what that cutting force will look like for this type of machining operation. Those green dots you see on those bottom two plots is a stability metric we use that says, is this cut stable or unstable? That stability metric can change based off my process parameter selection.

So because I've selected this spindle speed, this axial depth, radial depth of cut combination, what this map is telling me is that cut is going to be stable. There is no guesswork here. We took a measurement. Now we're going to use that measurement in our CAM, and I can show that this is going to be a stable cut. OK, let's try another one.

Now, I'm going to increase my axial engagement. Earlier, it was 50% or 50%. Let's bump it up to 75%, so we can engage more of that flute. Now we'll keep the spindle speed the same, and then we'll run a second simulation on. So we'll let that simulation run. It takes just a few seconds here.

Now something interesting has happened. I picked a point that is in an unstable region of my stability plot. Well, how do I know it's unstable? Well, go to our cutting force and our tool vibration plots one more time.

And as I take a look at these plots, I've noticed that stability metric has changed significantly. And if you remember that cutting force profile from that last figure, they look very different. Why do they look different? Well, this is an unstable cut.

So we've built in simulation into this tool that can show you via the cutting force and the tool vibration, the difference between stable and unstable cutting zones. Now, we'll see this being used in that aerospace panel case study.

OK, so let's start with supplier A, tool A. In this case, this supplier did have a cutting tool recommendation wizard. We use that wizard, and we prescribed, OK, here's the type of tool that we're using.

You can match the skew. Here's the material that we're cutting. A lot of them let you prescribe the material, and now it's going to give me a recommendation. In this case, this cutting tool recommended-- or this cutting tool advisor recommended a spindle speed of 6723 RPM at a speed of 268.2 meters per minute.

As a matter of fact, when we tried this cut number, the first thing we did was simulate it. We saw that this cut was going to be an unstable cut, but hey, we could be wrong. It's right at the limit. As a matter of fact, when we started our machining trials, this was absolutely an unstable cut.

So given this cutting tool supplier's recommendation, at a radial depth of cut of 25%, axial depth of cut of 75%, we respected their feed per tooth values. In this case, it was about 117 micrometers per tooth. We had an unstable cut.

So naturally, what do most people in the field do when they run into this situation? Your natural inclination is almost always to slow down. And that's exactly what we did. So how do I find a stable cutting region? Typically, your operator is going to say that cut is unstable. I need to now adjust my process parameters.

One really easy way for them to do that is a very convenient button on my machine tool that says -10% on my spindle speed. And that's what we were able to do in this case. We slowly adjusted our spindle speed down until we had a stable cut. And so you can see those updated process parameters in the table on the right-hand side.

In this case, my spindle speed was 6387 RPM. We respected their radial depth of cut and axial depth of cut recommendations. We did leave those the same. We left the feed per tooth value the same, and the end result was a stable cutting operation.

Through our machining dynamics add in, I could have told you earlier that this was going to be a stable cut. However, I could have told you that the recommendation we had prior was going to be an unstable cut and so that we shouldn't have used it to begin with.

And so what we wanted to do here was first say, OK, let's see what that total cycle time value is when I use my supplier recommendation. And so the video, you see on the right-hand side is a time lapse video of us machining that setup to-- for the panel. And you'll see that right now, I think it's in the pocketing operations. The video is playing that just showcases the cutting process.

So in the case of this part, the total cycle time was about 52 minutes and 8 seconds. Now, I want to remind the audience, we're not trying to optimize for cycle time completely just yet. We'll talk about how we can do that a little bit later on. But in this case, we just want to know, do the recommendations I get from a supplier work, or do they not work?

So in this case, this first recommendation didn't quite get us where we needed to be. So there had to be some of that manual intervention you heard about earlier. That manual intervention is something that happens quite frequently in a shop floor environment.

And so we did intervene manually to find a stable cutting zone. However, what if I wanted to try and optimize this with machining dynamics? I see the map on that top left panel, and I can see my cutting forces on the bottom left panels.

So what we're going to do here is we're only going to optimize for spindle speed. We're going to keep it simple. We're not going to change the radial depth. We're not going to change the axial depth.

We're not even going to change feed per tooth. We can change all of those parameters using this machining dynamic strategy.

But the first thing we're going to do is optimize for spindle speed. So the machines that these were on had a maximum spindle speed of 12,000 RPM. So what am I going to do?

Well, the first thing I can do is in my MSC add in, I can simulate the point that I want to run, which is what we did. Let's look at the bottom left plots. I have a cutting force that looks stable.

I have a tool vibration that looks stable. My stability metric is green, which means that cut is going to be stable. And then, of course, I changed my toolpath. Or my process parameters, that is, for that 1/2-inch cutting tool.

So now you can see our feed per tooth value remained the same. Our radial depth of cut and axial depth of cut values remain the same. However, the only thing we optimized for was speed. And I only measured one tool and applied this to one cutting tool.

What is the result? Well, the result is my total cycle time is now 38 minutes and two seconds. I've reduced my cycle time by 27% simply by optimizing spindle speed.

There are plenty of opportunity for additional optimizations. However, we'll see what that looks like a little bit later on. So we'll let this video play here for just a couple more seconds. And you can see that adaptive clearing operation and then that final kind of chamfer operation for the part.

OK, let's look at supplier two. OK, supplier two's tool recommendation platform was a little bit different. So the last one recommended a 25% radial depth of cut. This one went a little conservative with a 10% radial depth of cut. The axial depth of cut remained the same, about 75%

However, their recommendation was the spindle speed of 2785 RPM. So even for aluminum, that's quite slow. However, we double-checked this with both their tool recommendation platform and their handbook, and this was the recommendation that they had for this cutting tool in this material. In this case, the material, as you might have seen earlier, is aluminum 6061.

OK, with this supplier's recommendation, yes, I get a stable cut. However, what is the implication here? My total cycle time now is 5 hours and 15 minutes to make this part. That's a significant amount of time.

Now, if you're using some of these platforms and these are stable cutting parameters, maybe you're happy with those parameters. But a lot of times, especially when I've talked to customers, I've worked out in the field. There is a lot of these parameters can work. But we really want to try and optimize.

Well, how would I do that? So again, in this case, we didn't optimize for anything else other than spindle speed. Now look at the results.

In this case, we took our cycle time from about five hours to now about an hour and a half total cycle time. We reduced our cycle time by 71% simply by optimizing spindle speed. We left our radial depth of cut the same, axial depth of cut the same, feed per tooth, the same as the supplier recommended. And you can see in our stability plot on the left-hand side, we knew that cut was going to be stable.

Now, you might be asking, well, wait a minute, that map is all the way. Those unstable zones are so far away. Couldn't we increase our radial depth of cut? Yes, we can.

Couldn't we have increased our flute engagement if the part was a little bit bigger? Absolutely, yes, we can. However, we wanted to just focus on the spindle speed so you could see the value of even optimizing something like spindle speed for your machine tool.

OK, now we get to our final tool. And this one was pretty interesting. So this tool recommendation platform recommended a radial depth of cut of 15% Now, the first one was 25%. The last one was 10%. This one was 15%-- so interesting. Each one is giving us a slightly different answer for how you should use their tool. OK, axial depth of cut was the same.

Now their recommendation was max spindle speed. Well, what use is that for me? If I have a spindle that's about 20,000 RPM, can I run this part at 20,000 RPM? Maybe in the case of the machines that we have here, the max spindle speed was 12,000 RPM.

So OK, we picked 12,000 RPM. And so what do we notice? Well, my spindle speed is already maxed out. And these last two examples we talked about, I mentioned that we're there to optimize speed.

Well, if my recommendation is maximum speed, what other knobs can I turn? And this is where the real power of machining dynamics comes into play.

So we'll watch this video here for a couple more seconds. So in this case, the total cycle time was about 48 minutes and 27 seconds. And again, you can see that pocketing operation starting on the right-hand side. We'll let it play.

And what I want to ask the audience is, what else could I optimize? So as I go to my actual optimization routine, we'll take a look at it here on this next slide. We're going to optimize our feed rate. We can optimize our radial depth to achieve a reduction in cycle time.

And so now you can see the difference between that last feed rate and this feed rate. So we increase the feed rate. Spindle speed is already at a maximum value, but now I increase my radial depth of cut a little bit more.

Now you might say, well, well, did you just-- was it trial and error? Absolutely not. If you look at that left-hand side, you can actually see we're actually kind of pushing the limit of what my map tells me I can do.

If I were to increase my radial immersion percentage, you would still see-- you would start to see those stability zones drop lower and lower and lower. And that's just the nature of increasing my radial depth of cut. So in this case, we just increase the radial depth of cut to a point we were comfortable with, in this case, 25%, and then selected again that same axial depth of cut spindle speed combination to really push the limit.

Now I say, push the limit. My simulation is telling me that this is going to be a stable cut. If I were to increase my axial depth of cut slightly, that cut now might be unstable. If I were to increase my radial depth of cut slightly, that might be unstable, but I don't have to guess.

I don't have to wonder, well, will it be stable? Will it be unstable? Somebody make sure to write that down and record what the response was.

In this case, we did it all through simulation. We did it all in the CAM workspace, and I'm able to confidently select process parameter points that let me make a part as fast as I possibly can. So by optimizing my feed rate and my radial depth of cut, I achieved a 28% reduction in cycle time. So in this case, this part took about 34 minutes. So let's think about what we just saw.

We looked at three cutting tools. We looked at these static handbook value recommendations or tool wizard recommendations that suppliers provided. And I always want to say suppliers provide really good recommendations.

As you saw, a lot of those recommendations largely were stable cutting zones, which is great. However, those stable zones aren't quite optimal for the machine.

Now, why is that? Well, you heard it earlier today. The combination of the tool holder and machine matter. My stick out length of those tools matter.

Now, what if one tool was significantly longer than another tool? Am I going to get the same performance? Probably not going to get the same performance.