CAM for 4th axis trial

Trial, as in actually cutting some metal.

First of all, change the origin to something more convenient. I'll be able to pick up the sides and the top face of the stock with the 3D probe, then set the origin at the top as shown.

Then change the toolpath type to 2D Contour, rather than 2D adaptive. I plan to use my Korloy indexable face mill (with uncoated, loominum cutting inserts) rather than the long series carbide end mill. No reason or need to use poncy toolpaths here, as I'm just shaving the stock down to a simple flat - these mills are design for that! Again, make a single toolpath, then simply create a circular pattern of 4 from it:

Be rude not to simulate it, to check it looks about right. I've changed the model and CAM orientation to make it more natural.

The g code has to be generated by a different version of the generic Fanuc post processor that creates the 4th axis (ie "A") coordinates. Up until now I've been using a simple 3-axis post processor that only generates X, Y & Z coordinates.

The post processors are freely available from the Autodesk website and their customisation is encouraged. For the 4th axis g code, the required post processor (aka post to the big boys) is the one described as "FANUC - Inverse Time and A-axis". No idea what this "inverse time" stuff is about but hey. It pays to change the name and save it safely in your cloud posts otherwise you may lose them if an update is posted or you lose your local copy. That's a lesson I should have anticipated when I wiped my laptop back in November.....

The posts are "simply" written in Javascript. Although I'm no expert in this, I can just about figure out what they are up to and was able to make some modifications to suit the Newker controller:

• The Newker controller doesn't do a G28 move properly, so I added some moves at the end of the code to take the table to specified coordinates. These were developed by Timothy Dykes (aka "At-Man" on Youtube) and I was able to implement them without drama. G28 is intended to move the table to a convenient position at the end of the program, eg to bring the work close to the door so you can actually reach it easily.
• Similarly, I added a "G53 G90 Z0" move to ensure the spindle is withdrawn safely - I couldn't use the same code as the last changes.

When you call up the post, the user configurable items show up in the panel. So in this case I have disabled the "home position" move - I don't want the table and rotary table to fly about at the end of the operation. The current default values are machine coordinates of 200mm (X) and 390mm (Y), although you can change those from the panel:

Here's the beginning of the modified post processor itself. This is intended to be suitable for the Newker 990MDc controller with 4 axes. The editor used by Fusion is Brackets, which is an open source editor that supports Javascript amongst others.

Here's the beginning of the g code it generated. You can see that in line 14, the A axis is told to go to zero (units are degrees): 

Once Fusion has generated the g code, it automatically opens it in Brackets. I then save a copy to the USB flash drive (UFD) and carry it out to the machine - once I've put on my rubber underwear.

But first, I need to sanity check the tool offsets etc by checking the setup sheet. In this case there is only one tool, so it shouldn't be a big issue (haha). However, there is a fair bit of info in the setup sheet so it is sensible to sanity check it now, rather than stress test the rubber underwear later.

The 4 operations are identical, apart from the actual A coordinate. Lots of duplication.

So, to run the part:

Set up stock and WCS origin:

• Select the 3D probe tool from the tool table (using MDI).
• Insert said 3D probe tool into the spindle.
• Change to G54 (ie work coords, not machine coords).
• Position the probe on the top of the stock (Z = 0) and zero the Z axis.
• Position the probe on the end face of the stock (X = 0) and zero the X axis.
• Probe the sides of the stock and then zero the Y axis at the mid position (Y = 0).
• (This should ensure that the spindle and A axis are coincident).

Machine the part:

• Remove the 3D probe.
• Fit the 50mm face mill.
• Change the tool number to the correct value for the face mill(!!!) using MDI.
• Manually jog the spindle down to just above the stock to sanity check the WCS and tool length info looks right.
• Check work is secure.
• Stand by with the WD40 (lube).....
• Load up the program and run it.