In this lesson, we'll learn how to identify a 3D step-over amount for a specific tool. After completing this lesson, you'll be able to define scallop, illustrate scallop versus step-over, and modify toolpath parameters to minimize scallop. For this next lesson, we want to upload the supplied file, scallop versus step-over. We're going to be exploring this as well as the circular 3D milling file that we were looking at in a previous lesson. The topic we want to talk about here, is identifying what a 3D step-over should be for our specific geometry and how to pick the right tool. So the first thing that we want to do, is we want to take a look at the 2D contour operation that's in this file. We're going to simulate it and we use the go to next operation. By viewing this from the front. What we see here is something called a scallop. The scallop is going to be the material or the wave shape that's left behind when we're using a circular tool. This is going to be driven by the step-over of the tool. In this case, we're just talking about a simple 2D contour that stepping over just in x and y. But this applies to our 3D geometry as well. So we want to make sure we first boil this topic down to 2D and then we can explore how it affects our 3D parts. In general, there's going to be a point of diminishing returns when we talk about setting a step over value. In general, that is going to be somewhere around one-tenth the diameter of our tool. Now, in our case, if we take a look at our operation, the tool that we're using is an eighth inch ball and mill. If we take a look at this on a calculator, that's going to be 0.125 diameter and we're going to divide that by 10. This means that our step-over, if it's any less than 0.0125, it's really going to be a point of diminishing returns, where we're spending a lot more time machining but we're not really getting a return on the quality. Now, of course, you will get a better quality finish but just keep in mind that there is a certain point where that doesn't make sense. On the low end of this, we can take that same 0.125 tool and divide it by three and on the maximum side we would want to go over a distance of 0.0416. Now, this is going to be used for softer materials like wood and things that we can hand sand after the fact to smooth out. This means that it's going to take a lot more time for us to have a finer resolution step over to machine those materials where we're really not going to get the same kind of tolerances that we would machining aluminum or steel. So again, there's this point of diminishing returns and in general we're going to be shooting for about the one-tenth to one-eighth range. So somewhere in the 0.15-0.125 range for this tool. So let's see what that looks like in our 2D contour operation. I'm going to duplicate this, then I'm going to edit the duplicate. We're going to go into passes and inside here we have 16 finishing passes that are stepping over at 0.125. So we're going to set this to be 0.125 and say okay. Notice that this is a much tighter grouping and if we simulate justice operation, we're going to go to next and view this from the front. We can see that we really aren't seeing any scallops here. So as we look at this tool path, we get a nice smooth finish, and we're not viewing any of those scallops. If we go back and we edit this tool path and go into passes and instead of going the 0.125 and we go to the upper end of it. 0.416 and say okay, then again once it calculates, we simulate this, we use go to next, and we'll view from the front. You can see that we are getting that slight scallop. We still have nice flat spots between these areas but we are seeing this slight scallop in between. This is going to be something we would use on again a wood part something that we can go back and we can sand relatively easily. Another factor that we want to keep in mind when we talk about deciding what our step over should be to minimize that scallop geometry is going to be the diameter of the tool. Now obviously, we're looking at an eighth inch diameter. So we're dividing that by eight or 10 to get what our maximum step-over should be. But is eighth then should going to be the right tool for the job? So let's take a look at our circular 3D milling example. Let's take a look at the geometry on the screen. Is larger, fill it on the bottom, is a half-inch radius, which means that it's a one-inch diameter. So in order for us to cut this geometry, there's really no need for us to have such a small tool as an eighth end mill. We could go all the way up to a half inch ball and mill or larger, assuming that the radius of our tool is less than the radius of this curvature that we're cutting. So what that means is, we can take that larger tool, that half-inch or even if we went all the way up to a one-inch, and if we divide it by eight or 10, we're able to step over a much larger amount to cut the same resolution without those scallops. But now that we know that, let's take a look at the spiral cut and let's modify its parameters and take a look at this step-over that we used. So in this case, we use this step-over of 0.0025. This is a much too fine of a step-over. So if we go down to 0.125 and we rebuild that, this 0.125 is going to be a little bit closer to what we want to see if we were cutting horizontal geometry. So we'll control select adaptive and we'll simulate this. We're going to simply jump all the way to the end and take a look at the final result. So as we look at the final result from a front view, you can see that as we get closer to horizontal, that step-over is getting a lot closer to being a smooth resolution. Same thing that we see on top, that step-over looks pretty good until we get to these vertical edges. So what this means is, as we start to plan it out, we really need to be careful with not only the step-over, a mount of the diameter of the tool but also the specifics for our geometry. Now, there are tool paths such as contour that allow us to go around this part and it can change the step-over amount or the step-down amount in this case based on the curvature. I can increase or decrease that and we can also focus on specific areas and allowing it to modify those parameters will get us a much better cut. But these are going to be the general things that we want to keep in mind as we start to think about, actually populating some of these parameters. We don't simply want to go in and just put a really small number so that it looks good on the screen, we want to actually think about this and calculate this. Again, the rough range that I would look for is somewhere between a third of the tool diameter down to a tenth of the tool diameter, somewhere in that one-eighth to one-tenth is usually the sweet spot and anything above that you're going to start to see diminishing returns and you're just going to increase the program time. So this is about where we start. Again, that always needs to be done through testing and validation. We need to make sure that we're not just making a 10 hour long program, when it could be done in two hours with pretty close to the same results. So I strongly urge you to go back in and start playing around with the different operations that we've already taken a look at, for doing our 2D contour and our ramp, then exploring things like this spiral radial and more spiral here and then going into our scallop versus step-over and playing around with these values and maybe even going in and picking some different tools so that we can get an idea of how that tool diameter affects the overall step-over. Once you're done, of course, save these files and then we can move on to the next step.
