In this lesson, we'll identify 3D stepover for a specific tool. After completing this lesson, you'll be able to define scallop, illustrate scallop versus stepover, and modify toolpath parameters to minimize scallop. In Fusion 360, we want to start with this applied dataset, scallop versus stepover. We also want to make sure that we still have circular 3D milling open. First, we want to take a look at scallop vs stepover in the 2D contour operation. If we take a look at this from the front, we can see that this ball end mill, that's machine the top of the part has left a bunch of ridges. This is what we call scallop and this is something that we often need to work hard to avoid on complex 3D parts. When we're machining 3D parts, we want to minimize the amount of scallop, but there's always going to be a fine line between the amount of stepover the tool has and any diminishing returns. The more we increase that stepover, the more scallops we'll have on the part. But when we make it so small that we have so many passes, we essentially are taking a very small cut each time and we're increasing the program time exponentially. So in this lesson, we want to talk a little bit about how to minimize that and what sort of things we should be looking for. The first thing I want to talk about is in general what kind of values or numbers should we be looking for. If we go into this operation and into the 2D contour, the value that we're looking for, in this case, is the stepover. We're dealing with an 8th inch ball and mill. And right now this step over is 0.125. So this means it's moving over its entire diameter each pass, and that's why we have such a large scallop. When we're talking about what number we should be putting in here for the scallop, it really comes down to what the material is and what any post finishing operations or manual operations might be happening in general. In general, about 1/10th of the diameter is the point of diminishing returns. So for this 8th inch ball and mill that would be 0.125. So let's go ahead and put 0.0125 in there, regenerate this and take a look at the results. Now obviously it didn't step over nearly as far, but you can see now we have this nice flat section and everything looks like it's been machined pretty well. So we know that about 1/10th gives us a pretty good result. But what other values could we use to get a decent result without spending so much time on the program? Well, for this 8th in ball and mill going down to a 10th was 0.125. A third is probably the upper limit of where you can go on some materials. So in this case, a third of the 8th inch ball in mill would be 0.4. So I'm going to put .04 in here and allow it to regenerate and take a look at the results. So now we can see we still have a mostly flat section, but we've got these little bumps right in the middle. If we rotate this around, you can see what's left behind by that operation. So this 1/3rd value of the end mill, this is likely something that you would use on softer material. Maybe if you're machining foam or wood that's going to be used as a buck or a mold for something else. Something that you can easily hand finish that might save you a lot of programming time, especially on a large part to only use a third of the step over rather than a ten. Generally for aluminum parts, I would go to 1/8 or 1/10 of the diameter as a good rule of thumb, but the curvature is going to determine what that value is as well. And what I mean by that is, we're really looking at a simple example of a flat part. So this is the most basic example of the part stepping over each time. But if we go back to our circular 3D milling example and in this case, let's suppress the radio operation and let's bring back our spiral operation. And the spiral was probably one of the worst results out of these three that we looked at. So if we regenerate it, we take a look at the results, we should see that it left a pretty big jumps or pretty big gouges in the park. Now, this is what we're talking about when we're looking at the scallop of the tool. So if we want to make an adjustment to this, knowing that that roughly 1/8 to 1/10 of the tool is about the sweet spot, let's go ahead and modify the step over to be that 0.125. We're going to say, okay, allow it to regenerate and take a look at the results. So this value is much closer to that final. And while this worked pretty well on those upper and lower sections, when we got closer to those vertical walls, we can't count on the traditional stepover value. Because now we're getting farther and farther away from the curvature of the tool and we're really using more of the side, which is more like a flat and mill or a ball and mill. So in cases like this, we need to have a very specific operation, one that controls not only the stepover value, but the step down value. And can really take a look at it in relation to the curvature that we're working with. Now let's go ahead and suppress the spiral operation and let's bring back our radio operation. When we were looking at our radio operation, the definition for radio was based on an angular step, not a numerical one. So if we come back in and we take a look at the definition, you can see here that we've got 1 degree up to 360 degrees in 1 degree increments. Also notice that there is a minimum stepover value. The minimum is set at zero by default, but if we put in a larger value like 0.04, that 0.04 is what we used as sort of that 1/3 upper limit where we can go back and we can hand finish something. So as we can see the results here are now showing a lot of these different scallops on the part. They're not major, so depending on what the purpose of this part is, it might be an okay surface finish. Let's take a look at what the machining time is and in this case it's nine minutes for this result. If we go back and make that change and set this value back to zero, allow it to regenerate and take a look at the new machining time, we can see exactly what the difference is to get a much closer to finish part. So you can see we've gone to 15.5 minutes up from about 9. So while this is just a small part in a small example, you can see how these changes are going to be things that need to be planned out based on part you're working on, the operation you're using, the tool that you're using. And exactly what your requirements are for that surface finish. Now, I will say with this specific example, again, the part was custom tailored to highlight some of the weaknesses in some of these operations. But I should also mention that we're using a relatively small ball and mill. All the curvature on this part is fairly large, which means that we could go to a much larger tool. Which means that we could take larger steps because we're looking at an eighth or tenth of the diameter. So if we had a half inch ball and mill, that would cut this just fine. We could step that over quite a bit more. While we're here, let's go ahead and make sure that we do save both of these files and then we can move on to the next step.
