If you're looking to make detailed and complicated components out of carbon fibre like these quadcopter parts.
Really, the easiest way to do that is using CNC machining.
Fortunately with the new generators of light duty CNC routers this has become more affordable than ever.
However, there isn't an awful lot of information on how you go from your original design,
through to setting the feeds and speeds and really getting the most out of your CNC router.
So whether you already have one or you are looking to invest in a machine, this video is for you.
To get started with CNC machining, the first thing you will need is a CAD design package to design the parts.
We are using the excellent Fusion 360, which amazingly at the moment is offered free of charge to students, educators and enthusiasts.
We are then going to use the in built CAM functionality within Fusion to generate our tool paths and then the G-code.
The G-code will then be interpreted by the UCCNC software which came with the Stepcraft router to control the machine itself.
In case you are not familiar with desktop routers I am briefly going to go over what they are all about.
We have a spindle here which is a router spindle that does all of the cutting work of the carbon fibre,
so that has a carbide cutter mounted into it and that physically routes out the material.
To control that, we have a 3 axis machine here.
So we have control on the z-axis, which is the vertical here.
Then the x-axis which brings it across, and also then y-axis down the length of the machine.
Essentially we can position that spindle anywhere is this working area.
Now to get control of that the machine is run on what is called G-code.
We are going to show you how to generate that now.
We already have the model of the component we want to produce drawn up in CAD.
You can see that here now.
Here is the model and here is the design environment of Fusion.
If we click on the top corner here we can go into the CAM settings
and that gives us all of the manufacturing options which will control CNC machines.
So if we take a quick look we will just create a new set up here.
The first thing is it asking for is the model orientation.
So if we click on that and then click to select the z-axis.
So the z-axis is the vertical axis so we will click on this edge there.
Then on the x-axis that can be across that way and then it will automatically work out
what the y-axis would have to be from there.
So then we go into the stop tab at the top and because we are actually cutting this component from 1mm material
we can set the top offset so the extra material in the stock to 0mm.
That gives us a 1mm component out of 1mm sheet.
So we will click okay and there we have the setup and now we are onto the machining operation itself.
So it is a 2D operation it is just a profile and then we will go down and it is a contour machining operation.
So it is just machining the outer edges.
So first thing we need to do is select a tool.
I've already got these tools programmed into the system but what we are using is a PCB cutter.
This a 1.8mm PCB cutter so you can get right down to 2mm holes or radius'
and you can see we have just set the dimensions for that tool up so the length flutes,
the length of the shaft, the diameter of the shaft.
And it is very, very quick and easy to add new tools as and when you need them.
So we will click okay and that will bring in the feeds and speeds that we have already been set for that tool.
Finding the best feed and speed to set your machine to can be quite tricky.
What we suggest doing is play it safe, set your feed rate,
so the rate at which the cutter goes through the material very slow,
something around about 500mm per minute and the plunge rate slower still.
That is the rate the cutter actually plunges into the material itself.
That is something around about 50 - 100mm per minute.
Then the spindle speed should be a fast as it can go.
Now this will wear the tool slightly more quickly, but it takes a load off the machine,
and will give and very, very accurate cut.
As you gain experience in the way that your particular material is cutting,
you can increase those rates until it starts to sacrifice some of the accuracy or excessively load the machine.
With all of the feed and speed rates inputted,
we are going to go onto the geometry tab on the top here and then select all of the edges that we want to cut.
So, you can see all 39 chains there are selected.
Then we are going to add tabs on to the part.
Now the tabs are, you can see here, small linking components that actually keep the centre of the material attached to the stock material.
The purpose of those is when machining so that these small parts don't fly out of the part and maybe foul the machine or potentially break a cutter.
There are other ways you can secure it down.
A common way to do it is to use double sided tape over the reverse of the material and then firmly attach that down,
and again it stops those components from fouling the machine.
So to set the tabs up we just click on the tab option here,
set the width that we want the tab to be, they can be very, very small.
So we are going to set 0.5mm and then the tab height I am going to set that at 1.5mm.
Now you will see a little bit later why 1.5mm is the height I am setting.
Then the distance you can play around with different distances.
I am going to go for 25mm separation.
That looks pretty well spaced, everything seems to have something attaching it.
You might choose to manually control where those are as well.
So we will click onto heights and in heights we have got the clearance height,
so that is the height at which the tool clears all of the material.
The retract height which is between operations so when it goes from one section to the next.
Then we have got the feed height set down at 2mm.
That is the point at which it starts its cutting operation.
Top height at 0mm which is fine.
Then the bottom height we are going to set it from the stock bottom minus 1mm
and that will give us a cut that goes cleanly through the material.
You want to drop the tool right the way through the carbon and into the waste material underneath.
So then on passes these will all be fine for what we're doing,
but you might choose if you were cutting particularly thick material, multiple depths.
The purpose of multiple depths is your tool actually drops down into the profile, starts machining around but doesn't go all the way through.
It might drop maybe 1 or 2mm at a time and conduct the cut.
The purpose of doing that is to stop the tool from getting excessively hot
or to take load off the machine and on thicker materials anyting over, probably 3mm you would be looking to do multiple cuts.
On thinner materials like this, certainly 1mm, you will get excellent results with just a single pass right the way through.
We will just take off the multiple depths on there.
Linking, that is all fine as it is in stock settings so we will just click okay and that will generate our tool path.
So we can actually see the tool path now and you can actually see the tabs are these steps here
and you will notice the reason why we set them to 1.5mm is because the tabs go from that bottom line which is 1mm through.
So then we have got 0.5mm into the material itself.
We can actually click on simulate here and see the tool itself and the path that it takes and watch the machining operations.
So that is the tool and it is just following through the path.
It is quite a nice way to just preview whether there is going to be any problems or it is doing it in the order you expect.
So that is all looking fine and we can actually post the process now,
so generate the G-code which is this button at the top.
So we are using the UCCNC post processor and we are just going to make that, this is the frame lower section.
So we will just name that frame lower and then click on the post.
Choose the name for that frame lower, save.
That is the G-Code itself so we will run that in the UCCNC software shortly.
We have got a choice here of some of the sheet materials available from our factory.
Here we have got a 0.25mm sheet which as you can see is very, very pliable.
These range right up to sheets at 3mm which are suitable for very structurally demanding applications.
For this project 1mm sheet will be absolutely perfect.
The machine has this sacrificial bed that i have attached on using double sided tape.
This is a spoil board or a waste board that the cutter can drop into and carve through without damaging the bed of the machine itself.
To attach the carbon we are just going to use wood screws into the spoil board in the corners and that will hold it down
and then also, although not necessary I am going to put some spray mount onto the back of the sheet,
which on thin sections of carbon, below 1mm, it helps just to stop the carbon from lifting during the machining operation.
We are going to fit a fresh cutter into the machine,
so I just lock out the spindle and undo the collet here
and that will allow us to withdraw the old tool and then just reverse the process to put it back in.
These PCB cutters that we are using really are superb they are designed for cutting PCB, which is fibreglass and resin
but in composition that is very similar to carbon fibre making them absolutely ideal.
We have opened up UCCNC this if the software that actually controls the machine and then
we have loaded the file that we have just generated and we can see that on the screen here.
So the next thing to do is position the machine onto our work piece.
So looking at the machine itself we need to bring the head onto the centre of the tool path.
So we will just control the machine down.
So you can see this yellow marker in the centre here.
That is indicating where the centre of the tool is.
So if we click 0 all that is its intial reference point.
Now I have set the origin to be in the centre of the stock so if we just position the machine into the centre
and then lower the tool head and then once we get close in on the position we want to reduce the jog feed to a lower rate
so we can be more precise with the action.
Once it is almost in position and almost touching the surface.
Set the jog speed to its lowest setting and then very, very slowly bring the tool down.
A piece of paper helps because as soon as you start to see it pinch you know you are close enough to the surface.
That is just gripping it there so that is fine and then we will set the 0s for all of the axis' on there.
So we have got the centre set now in the stock but it is always worth while (just increase the jog feed there)
It is always worthwhile doing a quick check to see that the tool itself works within the stock material.
You can do that just by scrolling this up and just checking once it gets to the edge of the tool path that you are still within your material.
Which you can see there we are so we have got no problem.
Just increase the jog speed up a little bit more to do this a bit quicker.
So we will go over to the far side there, and you can see once again the tool is off the part and well within the material.
Likewise for the bottom there that is the same.
Normally I would use the dust extraction that is built into the machine here,
but today I am going to start the cycle without the brush in place so you can see what is going on.
The spindle can be controlled by the software or manually.
Today I am just going to do that manually.
So we just switch on the controller and then set the speed which is full speed and then press go.
And then all we have to do now is click the cycle start in the software and the cutting will take place.
We can now see the cutter following a path and how easily it cuts through the carbon fibre sheet.
To keep dust and chippings down we are using a vacuum cleaner.
While not ideal this provides a better view of what's happening.
Occasionally during a pass you will see the cutter lift slightly and resume the cut.
This is the operation where the tabs are being left in the stock to keep the off cuts in place.
With the brush fitted and local extraction turned on you can see how clean the cutting operation becomes.
The dust extractor is an optional extra from Stepcraft but one that we strongly recommend if working with carbon fibre.
The footage has been sped up here, this particular cutting operation took a little over 3 minutes in total.
The machine would be capable of faster cutting speeds but as mentioned earlier this may compromise the precision.
With the machining operation complete we can home the machine and remove the sheet from the spoil board.
You will see clearly where the cutter and plunged through the carbon and into the wood below.
Despite this the board can still be used many times before it will become worn and require a replacement.
You can see that most of the tabs, the cut out sections have broken off when we peeled it off.
That is because we used spray tack to hold it down.
Any that are remaining you can just break out using a stanley knife
and then the small tags that are remaining can be quickly removed using a Perma-Grit file.
The residue that has been left by the spray adhesive can quickly and easily be wiped off using acetone.
Just checking the finished component against the original drawings,
we have managed to achieve a tolerance better than +/- 0.1mm.
So there we have it, a finished carbon fibre part.
If you have already got one of these machines I hope this video inspires you to make your own precision carbon fibre components.
Remember Easy Composites has a full range of carbon fibre sheets for you to be getting on with projects like this.
If you want more information on the Stepcraft machine that we have been using today we have put a link in the description below.
If you have not seen them already we have got lots of other videos on working with carbon fibre.
If you have enjoyed this video click like. If you want to see new videos as we release them hit subscribe.