Join Thom Tremblay for an in-depth discussion in this video Defining the toolpath, part of Fusion 360: Designing for Metal.
- [Instructor] With the setup complete, we'll begin to tell the machine tools how to move and what to cut. There are additional toolpath options but each of them will need to know what they're using to cut and what material they need to remove and what limitations need to be respected. I'll select the Setup to remind myself of the boundary conditions of the stock material. To bring the material down to the top of the part, I'll use a face toolpath. I'll go to the 2D pull down, select the Face toolpath and with each of these toolpaths we'll be presented with multiple tabs.
These tabs are Tool, Geometry, Heights, Passes and Linking. We won't necessarily need to modify all of them for each toolpath but we need to make sure that the values are appropriate in each of them. We'll begin with the Tool tab. I'll select the tool that I want to use. Fusion 360 comes with large libraries from vendors as well as sample tools. These sample tools are organized based on the material and the units.
I'm working with a part that's aluminum in metric, so selecting this library will bring up a very large selection of tools. We can filter the library very easily by selecting the type of tool directly or setting the operation. By setting face and clicking OK it will limit the tool options to bull nose, flat and facing tools. I'll select a 10-millimeter flat end mill and click OK.
When I do this, it will bring in the spindle speed, the lead-in, the feed rates, all of the information that are built into the library. If you find that a tool in the library is close to what you need but doesn't have quite the correct information, you can always edit the library tool and start building your own library. For a facing operation there's really no need to select Geometry because it will work off of the stock contours and use the Heights tab to set the bottom height of the toolpath to the model top.
The Passes tab we might want to make one modification. We might want to extend the pass a little more than the radius of the tool, so I'll extend each pass by six millimeters. I'll click OK and generate the toolpath. When the toolpath preview appears, note that yellow shows high-speed transition, green shows low-speed transition and blue represents the actual cutting toolpath.
Let's move to the next operation. The next thing I'd like to do is drill out the holes in my part. So, I'll go to Drilling operation and I'll see that in this case there are four tabs. I'll select the tool, going again to the metric aluminum tools, I'll go to Type this time and tell it that I only want to see spot drills and regular drills. I'll press enter to take those filters.
I know that the hole that I need to drill is five millimeters, so I'll select a five millimeter drill. When I click OK, I'll move to the Geometry tab, tell it that I would like to select the five-millimeter diameter hole. Now, keeping in mind that so far all I've done is cut off the top of the material, it's showing that it would still be moving at a feed rate into this pocket. It's also showing that the tool would not come all the way to the bottom of the existing hole, only the tip, so what I'll need to do is make some modification in the Heights tab.
The first thing I'll do is I'll set the top height instead of the hole top to the model top. So, the cutting operation will begin at the model top. I could set the bottom height for the hole at the hole bottom but what I'd really like to do is have this pass all the way through the part, so I'll use the model bottom and I'll tell it to put the drill tip through the bottom.
Let me set the bottom view here so we can see what the operation looks like plus I'll ask it to go one millimeter beyond the bottom. The last tab is the Cycle tab for drilling. Instead of having it do a rapid out drill, I'll have it do chip breaking, so it's doing partial retract and then returning to the material to cut it again. I'll click OK to generate this toolpath. The toolpath is very simple as it's a drilling operation and I'll repeat a drilling operation.
In this case, I'll use the same drill. For my geometry I'll select the large hole but I don't want this to really go all the way through. Instead, I'll set my bottom height to the model top. I'll also set my top height to the model top plus give it a little gap and the bottom I want to penetrate into the material one millimeter.
So, I'll set it at a minus one. What I'm going to be using this for is just a pilot for the larger drill bit and I'll change the cycle to just rapid out, click OK and Fusion 360 will warn me that the retract height must be higher than the feed height. So, I'll update that value and get just my touch of the drill on the top of the material.
We have to imagine sometimes that the material will still be there. Now what I'd like to do is do another drilling operation that will go all the way through, basically the same drilling operation as I did at first but with a larger tool, so I'll right click on the first drilling operation and select Duplicate. This will create a new drilling operation with all the same parameters and I can rename this 10 millimeter hole so I can keep track of this.
This is a good practice for all of these. I'll edit it, change my tool, finding a 10 millimeter drill, changing the geometry by deselecting the holes and selecting the new one but keeping the other options the same, so rather than having to change all of the heights information, I can just simply say OK.
Now, I need to this to happen after this drilling operation, so I can simply click and drag to change the order. Now, I want to do the last operation I'll do in this set up which will be an adaptive toolpath, in this case a 3D adaptive toolpath. Adaptive clearing allows the tool to stay engaged longer and helps with tool wear. I'll change the tool under the metric aluminum library again.
For this model because I have a three-millimeter radius, I use a six-millimeter bull nose mill with a one millimeter edge. I'll select the tool, it'll update the tooling, I'll go to the Geometry tab and I'll select the contours that I want to remain. I'll use rest machining and I'll set my heights so that the tool and its radius run down below the finished face, so I'll set the bottom height to model bottom minus one millimeter.
On the Passes tab, I want to avoid having the mill try to recut these holes that will be drilled, so I'll tell it to not machine cavities and because this toolpath is often used in roughing, by default it would be leaving a half a millimeter radial and axial stock, so I'll deselect that option as the finish isn't terribly critical on this part and click OK to generate the toolpath. Looking at the toolpath it looks like it will be stepping down a few different times, so I'd like to edit the toolpath to take a look at the roughing steps.
On the Passes tab, I see that the maximum roughing step down is set to 10 millimeters. I could go back to the tool library and take a look at the flute length but what I'd like to do is have it calculate its own maximum depth based on the flute length that's attached to this particular tool and using three quarters of its length by saying times .75 of the tool flute length value, so even if I were to go back and change the tool, it would still update that depth based on the tool that I did select, in this case that will be 15 millimeters.
I'll click OK and it will update the toolpath again. This time it will save one extra pass. To analyze how this operation would look, I'd like to select the Setup, go to the Actions panel and select Simulate. What this will do is allow me to walk through the process of machining this part in a virtual environment. On the Display tab I can choose different options. I'll revisit that in a moment.
On the Info tab, as I run the simulation it will give me the positional and operational information as though this were running on the CNC machine and on the Statistics tab it will tell me what the machining distance will be, what the machining time would be, how many operations and how many tool changes are required. We could combine one of those tool changes but for now, we won't worry about it. I'll go back to the Display tab and tell it that rather than showing all of the toolpath, I'd only like to see the tail of the toolpath, the part of the toolpath just after the tool passes through and I would like to display the stock.
I'll begin the simulation to show you what this looks like. As it's cutting through, I'll see a portion of the toolpath and as it transitions to a new operation, you'll see that the coloration using this option changes. Let me stop and back this up. The controls will allow me to go back to the previous operation or even to the beginning. I'm going to change the material for my stock to ceramic. It might not look exactly like aluminum but it does give me a little better appearance.
I'll start my simulation again and I can control the speed of the simulation with the slide bar. So, here's my drilling operations and now my adaptive clearing. Another thing this will do is based on the speeds and feeds, and the type of tool, it will even show us a preview of what chatter or what surface imperfections might result from the way it's being cut.
Going back to the Info tab while this runs, we can see the information. I'll speed this up to finish it and we can see exactly what the part would look like coming off the machine after the first operation. There are two more setups that I would run on this part to cut the slot and to finish off the back side. In this video we used a few different toolpath types but of course, your design will have its own needs.
Just realize that whatever toolpaths are required to create your designs, it will have many of the same input requirements as we've seen here.
- Setting up parameters
- Joining components
- Animating and rendering the design
- Testing alternative materials
- Creating the setup
- Publishing and posting the design