Machining the X axis cover - finally. And a close escape!

The CAM for the X axis cover has been ready for a week or so but I've had a few distractions along the way, not least managing to bugger my back when putting some masking tape on the wall during some painting. WTF?? Bags of cement yes, tape on wall no.

Want to get this out of the way before I start to bugger about reworking The Shiz, removing the Newker controller and fitting the Centroid Acorn system instead. It should have been a quick job but things haven't worked out that way.

Last minute sanity check on tool lengths, using a 10mm (broken!) cutter shank:

Couple of issues fixed before starting:

• Many of the plunge and ramp feeds were pathetically slow. I corrected that in the tool library where possible. Values like 333m/min needed to be in the 1000-1500 range.
• The deep drill cycle was taking forever. Changed to peck.
• The 4.5 drill is now in an ER16 collet, so needed to change number to T05.
• I went for conventional milling on the chamfer operation. DCTTeacher suggested that as a means to improve the finish. Let's see how it works out.

Finally donned the rubber pants and went for it.

• The drill cycle was still pathetic. The feed height was 5mm, so it started pecking in air way before it got anywhere near the surface. And the peck depth was only 1.125mm, at which point it would retract and start again. Changed feed height to 2mm and peck to 3mm.
• The drill didn't break through. Although I'd selected "drill through bottom", for some reason I'd selected a 3mm offset (WTF??). Changed that now and also extended the hole 1mm beyond the stock bottom.
• The 6mm HSS slot drill sang a bit during the boring operation. But it WAS dry, so perhaps I shouldn't have been surprised.
• The main operation was the external 2D contour. As I recently removed the enclosure and didn't want to make a complete mess in the workshop, I tried to make do without coolant. However, the tool got hot and swarf ended up welding itself to the tool. Luckily I stopped the machine before the tool pinged but it was obviously a very close run.
• The chamfer was better on the top edge but still shit where it met the vertical face. I don't think I've got the feeds and speeds right and it's possibly not the best tool.
• The 2D adaptive for the bolt pockets left a 0.5mm "axial stock to leave". Stupid boy. So when I made the finishing pass (2D contour), it left a pip in the middle of the pocket. The countour operation doesn't clean up the horizontal middle of the face, only the vertical surface.

Here's the cutter. More like a stir welder than a cutter!!

And the result:

But despite all these issues, it actually went well. No lasting damage / evidence once the job was done.

I crudely snapped off the larger piece of stock from the tabs. Some saw / file work is still required to complete the job:

The pockets came out OK, apart from the 0.5mm pip I mentioned....

The hole chamfer was defined in CAD. Possibly a bit bigger than ideal, when positioned right next to edge chamfer.

I didn't do anything special in terms of cutter radius compensation so I was surprised and pleased to see that the 48mm diameter bore appears to be pretty darned accurate. Yes, I've checked these calipers with my slip gauges and they are actually pretty accurate themselves.

These were taken before I removed the work from the fixture

Job done!