In order to do any cutting on a CNC machine such as a ShopBot and to create tool paths
in Fusion 360, we need to be able to create a tool based on the actual cutter that we're
using.
For many of the processes a simple 2 flute Flat End Mill will cut fine.
Especially if you're cutting wood such as plywood.
There are other bits such a spiral bits and compression bits that you can use but using
a 2 flute flat end mill is a great place to get started.
Let's understand what the bit is made of.
When you look at the bit there are a number of different dimensions.
We need to think of the overall length of the bit, the length of the flutes which are
the cutting edges down here.
We also need to think of the diameter of the cutting edges.
The total tool diameter, the number of flutes.
In this case there are two flutes.
And we need to know the distance from the tip of the cutting edge to the beginning of
the shoulder.
The shoulder is where the tool starts to taper in.
So how do we make a tool like this in Fusion 360?
Once we collect all the data about the tool we can go to the manufacturer workspace and
then we can enter that data into Fusion 360.
So here in Fusion 360 let's go ahead and create the tool.
From the design workspace, we need to go to the manufacturer workspace.
Up in the top options you can click on Tool Library.
Your tool library will have tools that are in your actual document.
Here we have an Untitled document.
It has no tools it'll also have tools in your Cloud this is an Epilog Fusion laser cutter
tool that I've created.
It'll also have a local tool library.
In addition there is the Fusion 360 tool library that has sample tools and we can download
specific tool libraries from manufacturers.
You can create a tool in a document but then that tool will only be in that document.
You can also store tools in the cloud so they're accessible from anywhere.
The way to do that is to add tools to your local library and then we will back them up
in the cloud.
Make sure that you're not creating a new tool in your document.
Here we have a plus mark to create a new tool but we have Untitled selected.
We want to select our local library.
Here we can create a new tool in the local library, we can create new libraries as well
as separate and organize our tools.
Here I'm going to click new and first I'm going to create a holder.
A holder is not necessary but it's good to know how to create one so when you start doing
more complex operations or get in to 5-axis machining, you know how this works in Fusion
360.
The first thing we'll put in is a description.
This is an ER25 collet nut, the vendor is ShopBot, the product ID will be ER25 and then
we'll get the product link.
Here I have the link to the product, and I can copy that URL.
And then I can paste it here.
This information is not necessary but as you start to get more and more tools and holders
it's a good idea to have all the information in case you need to go back and find out which
specific tool you are using.
Then we need to enter the holder geometry.
We'll keep the unit is millimeters.
We'll click plus to have the first holder geometry height and for this will type 17
mm, the upper diameter will be 42 and then the lower diameter will be 42.
We'll create one more height, for this height it will be 3 mm tall, the upper diameter will
be 42 and then the lower diameter will be 32.
Now this represents the size of a collet nut on the ShopBot.
Again this is not necessary for 2D operations but it'll help us visualize and catch anything
that we might have at the wrong scale before we go out to post-process.
So now in my library I have this ER25 collet nut.
Now I want to create a new tool.
So I'm going to click plus and this time I'm going to create a Flat End Mill.
Now we're going to work through these tabs to put in the tool information.
For the description I'm going to type quarter inch Flat End Mill.
This tool is sold by Whiteside, product ID is 1014 and we'll get the URL We can copy
the URL from the browser then we'll move on to the cutter tab.
We.
want to make sure that the type is flat end mill.
And for this we're going to put the unit in inches since the tool is sold in inches.
We have a clockwise spindle rotation, the number of flutes will be too on this particular
tool, the material at high speed steel and then we need to enter the geometry.
The diameter as you can see in the image is the diameter of the cutter.
In this case is .25 inches.
Then the shaft diameter is calculated based on the cutter diameter so you can't enter
this dimension, it's automatically calculated.
The overall length can be entered but it is not used by Fusion to calculate anything.
So we can put in 2.5 inches since the tool is 2.5 inches but this is again not used in
2D cutting.
We need to have length below the holder but before I enter that, lets enter the important
number, the flute length.
The flute length needs to be one inch because that's how long the cutting edges on this
tool are.
And then the shoulder length is from the tip of the cutter to where the shoulder begins
to taper and on this particular tool it's the same as the flute length.
So we'll enter that as one.
Now the length below the holder needs to be longer than the shoulder and flute length
but not longer than the actual overall length.
So we'll type in 1.2 inches.
This way Fusion knows that some of the tool is going to be sticking out but it's going
to be different each time and that's why we will set the Z index when we do our cutting.
Then we'll move to shaft for a simple tool like this we don't need anything in the shaft
tab.
Click on holder again we don't need a holder for a 2D operation but we made our ER25 collet
nut so we can select it and then select holder.
Then we'll go to cutting data.
This is the most important tab when you were setting up your tool.
We need to set up the different feeds and speeds for our tool.
You can usually find these in the manufacturer's website and ShopBot has some recommendations.
For this tool I'm going to set in the default recommendations for ShopBot that then need
to be edited based on your material, your operations and your particular machine.
For spindle speed we're going to type in 18000 RPMs, in the ramp spindle speed will keep
the same, we'll type in 18000 RPMs.
The cutting feed rate we're going to put in 144 inches per minute, again this is a recommended
beginning setting from ShopBot.
The feed per tooth, lead in feed rate and lead out feed rate are all calculated by Fusion.
The ramp feed rate we'll keep at half of the cutting feet rate so we'll have it at 72.
The same for the plunge feed rate we'll keep that at 72.
Then under the passes and linking tab we can click the use step down box.
What this does is changing the default step down so if we click multiple depth in our
operations it will use this number rather than the default number.
Here we have a very small step down we want a larger step down.
The step down generally wants to be half the tool diameter, so here will type in .125 inches
which is an eighth of an inch since we have 1/4 inch bit.
Then on coolant it says flood.
We're cutting wood so we're not going to use any coolant, so click disabled.
Then scroll up click post processor, for post-processing we don't need any information here if you
were going to have multiple numbers of tools and you wanted to know which tool number was
which for tool changes you can change this here.
Then we'll click accept and now we have our tool and we can see it.
Now we can select this tool and holder and use it in our manufacturing workspace