2D Chamfer Fusion 360
Chamfering is a simple milling operation, but significantly affecting the appearance and functionality of the finished part. By bending sharp edges during milling, we shorten the time of manual finishing. In order to make the chamfer we do not need them on the model, but also their presence does not bother in any way, and may even be useful. First, we will check what the chamfering looks like if there are no chamfers on the model.
One of the ways to add a chamfering operation is to use the operation dedicated for this purpose. From the 2D menu, choose the 2D Chamfer operation.
In the first tab, as a standard, we have to choose a tool. We could use one of the tools from the sample tool library, but for training purposes we define a new tool.
Click the Select button to go to the tool library.
Click the New Mill Tool button to add a new tool.
In the General tab, in the Description field, enter the name of the tool – Chamfer Mill.
Let’s go to the Cutter tab.
Fill in the data as in the figure above and go to the Feed & Speed tab.
Fill out the data as in the figure above, and leave the default data in the Post Processor tab.
Let’s choose this tool and go to the Geometry tab.
Indicate the geometry shown in the figure above. We leave the Heights tab with default parameters. Let’s go to the Passes tab.
Compared to previous strategies, we have a new section here – Chamfer.
The Chamfer Width parameter is the width of the chamfer. This is the size of the chamfer, as if we were looking at it from the side.
The Chamfer Tip Offset is a very useful parameter. I will use an example. We want to make a 1 x 45 chamfer. For this purpose, we give 1 mm as the chamfer width and if we entered 0 in the Chamfer Width parameter, the tool with its tip (the lowest point) will move only 1 mm below the selected contour. And as you probably know, making chamfers with the tip of the tool (in most cases) is not a good solution. At this point, the tool is weaker, there is not much material and the flute easily crumbles. Therefore, it would be better to lower the tool a bit. And this is what Chamfer Tip Offset corresponds to. If, as in the example, you enter 1 mm there, the depth at which the tool tip will move will be: Chamfer Width + value from Chamfer Tip Offset, in this case, 2 mm below the contour. Now a question may arise, if we lower the tool, will not the chamfer be bigger? The dimension of the chamfer is controlled by Fusion 360. If you lower the tool in the Z axis using the Chamfer Tip Offset parameter, the system will move the tool in the XY axis so that you get the chamfer dimension entered in the Chamfer Width parameter.
The Chamfer Clearance parameter specifies the safe distance of the tool from the walls of the model. For example, if you chamfer an edge that ends at a wall, the chamfer will not be made to the end of the edge. The tool will end milling at a distance from the wall entered in the Chamfer Clearance parameter.
All we have to do is mark the entire contour, and the Fusion 360 will recognize where it can do the chamfering. Very useful function.
The other options in this tab as well as the next options were discussed in the machining of contours.
This is not the only way of chamfering in Autodesk Fusion 360. The next one will be discussed in the next post.