CNC'd aluminium jig

simpit · 14 June 2023 09:25

I am currently building a flight stand out of aluminium extrusion, and as step towards that I need a drilling jig.

I’m aware that there is only one other member who does CNC’d aluminium, so I want to document what I’m doing for reference.

This jig is to be milled from a 100x100x8 mm block of grade 5083 aluminium on the desktop mini CNC.

Here is the design I have settled on:

test_view.pdf (146.7 KB)

This design was created in FreeCad, an opensource cad tool which I am using.

I import the model into VCarve and convert to GCode, after setting up a spoilboard I began the cutting process.

My first attempt was to use one a 2mm 2 flute end mill, and as you can see from the image, the results were not great (no end mills were harmed in the making of this image).

The workpiece got very hot and the end mill had aluminium fused to the cutting surface as a result, chips were not being evacuated.

I have decided to take a different approach, generating the GCode with different software (The Path workbench in FreeCAD) because I am not a fan of VCarve, and I’ve sourced a number of different end mills.

As you can see from the pics, I have gone for single flute end mills which I am hoping will be more effective at evacuating chips and dispersing heat.

The end mills were sourced from https://www.shop-apt.co.uk/, below are the links to the end mills.

I have also sourced a long neck 1mm, 2 flute end mill to be able to do finishing work deeper in the workpiece.

CAM SOFTWARE

Originally used VCarve for CAM (Computer Aided Manufacturing) to convert the model into GCode for LinuxCNC but want to use something different.

Not a lot of OpenSource options that are available.

Have been playing around with PyCAM, which kind of works but is lacking features.

https://pycam.sourceforge.net/

Another option I looked at was BlenderCAM, which is a plugin for Blender, I found this to be a bit buggy and lacking in some features.

I have now settled on the Path Workbench in FreeCAD

https://wiki.freecad.org/Path_Workbench

I’ve also played around with Camotics as CAM simulation tool as well.

https://camotics.org/

davidN · 15 June 2023 06:49

Hey, thanks for sharing. I’m also interested in milling alu, so interested to see how you get on.

I have some experience with milling but by no means an expert.

The new endmills are a good shout. I’d imagine the one used is dull and the main cause of that awful looking cut. Curious as to what the speed of the spindle was and the feed rate?

I personally would rough cut the size required with a few mm extra on the sides. That way the end mill is only cutting on one side. Holding it down becomes a problem then… but you could maybe use double sided sticky tape if the feeds and speeds were right! Never used it myself but it’s an ‘old machinists trick’.

Lastly, lubricant when cutting alu is useful, a little dab of wd40 might help?

Looks forward to seeing mk 2!

simpit · 15 June 2023 09:32

I’ve been using MOLYSLIP - MWF cutting oil as a cutting lubricant for my drilling up to now, my first attempt (with the CNC) was completely dry, next time I will have some on the end mill and material surface.

I’m going to square off the workpiece in the CNC before making beginning the cut.

I’m also planning on adding a surrounding support structure as part of the design so that it will fit in the clamp without issue and be able to flip over without losing XYZ homing. I have no idea what the term for that is though.

simpit · 15 June 2023 09:50

I’ve come across this post on milling brass, with this SUPER helpful comment on fixturing (whIch I am going to attempt to use).

@CNCtechs, can I update the Desktop CNC toolpage to include brass as an acceptable material?

Mauro_Meneghin · 15 June 2023 10:49

A 2mm endmill is unlikely to cut through 8mm thick material because of the smaller flute length, it may end up rubbing trying to push down on the later passes.
What depth of cut did you use in the end?

simpit · 15 June 2023 11:02

From the first (and currently only) attempt, the end mill went down to 4mm before it started having issues.

The shaft diameter was also 2mm.

Federico · 15 June 2023 11:06

Brass is acceptable material for the cnc. Go ahead.

FrancisRJ · 15 June 2023 17:18

Hey @simpit,

I did another CNC project with brass:

In the discussions around that project @Kyle had posted a great resource about fixturing in CNC which goes into the ‘superglue’ method.

One problem I had was the super glue melting when the work piece got too hot. It happened when I was machining away quite alot of material in one go, just something to be aware of

simpit · 15 June 2023 17:56

Excellent suggestions.

I went with a different approach:

Annoyingly when I ran my gcode it missed the workpiece by about 4mm after touching off.

So I’m just trying to figure out what I did wrong.

FrancisRJ · 15 June 2023 18:43

If you are using freecad and the z height is the problem, I had something similar which seemed to be related to freecad turning on tool length compensation.

I fixed it by changing all of my tools to have tool number, I think #2, that tool does not have a z-offset set in the tool table in linuxcnc so the compensation doesn’t do anything.

There may be a better solution but that worked for me.

simpit · 16 June 2023 08:58

The issue was my stock was set at x-4 in freecad path workbench, but was not displaying this in the simulation.

It did however display it in camotics simulator, so I’ll be checking it against that in future.

simpit · 16 June 2023 20:19

Have squared off the stock for the next step.

The 6mm single flute end mill worked a treat, lots of chips, no heat, wasn’t even warm afterwards.

Used the precision square to get right angles with the clamps.

Some points of learning:

The stock wasn’t bolted down tight enough, with about 2mm of depth left it moved slightly.

I had to reposition the stock and touch off all over again. Of course I couldn’t get it to match up perfectly, was off on each axis by about 0.2mm.

The wasteboard was smaller than the stock, and as a result the last 0.4mm flexed down and remained uncut.

You can also see some of the support tabs, 4x4 mm

Fortunately I am left with a perfectly symmetrical sides for the clamp.

Feeds n speeds:

10k rpm, vertical and horizontal speeds will be added with an update.

Drop speed was 1mm/s, used a profile operation which wasn’t careful about dropping, some extra vibration when doing this.

simpit · 16 June 2023 20:36

The image below shows the support tabs, you can see the extra marks in the side from chatter as the mill dropped over the tab.

I don’t know if this is caused by the end mill having only a single flute or if it’s the drop in the profile operation.

The only issue this causes is finishing, so might consider starting from the bottom and moving up when doing a finishing run.