End Plate

I made another part from aluminium alloy.
There were a few lessons learnt here. The most exciting one was where I hadn't tightened the 16mm tool holder into its collet enough. I noticed the tool was cutting deeper than it should, so I paused the machine and set the z lower so it would cut higher.
I started again but it continued to cut deeper as it went. I stopped and adjusted the z value again. I assumend that something was going wrong with the Z axis drive of my machine. I continued to cut until the tool holder fell out and wedged over at an angle!
Fortunately nothing had been damaged, as far as I can tell, and the part had been cut oversize, where it went wrong, so it should be OK.
I had to stop there, yesterday. I came back this morning and tried again. I looked at various positions of the part on the computer and then set the x, y, z of the machine by touching the tool against already machined faces of the part, with a piece of paper. However, as soon as the tool started cutting metal again, the part came unglued. The coolant had unstuck the super-glue, overnight.
I pressed the big red button, took the part off, cleaned it up, machined a new area in the wood, with some islands to locate the part. It was a bit of a tight fit, so I hammered the part down to glue it down. This probably isn't good for my machine, although it is resting on a lump of wood.
I am happy with the finished part. I did have to hammer it straight again afterwards though.
Another thing, I have seen before, is where I am cutting a sharp inside corner ( or one the same radius as the tool radius ). On the finish pass, the amount of material taken off is quite accurate because there is not much deflection or vibration until it gets to the sharp corner. It then momentarily squeals as it cuts the entire corner in one instant. You can see from the last picture how there is a lot of deflection ( I gues about 0.3mm on my 6mm tool. A solution would be to change the shape of the pocket so that the internal radiuses are at least a bit more than the tool radius, or to use a smaller tool.

More Delrin parts

Some more parts were asked for, yesterday evening. I have made them and will go to the Post Office tomorrow morning and send them first class.
I made the round ones first. My 6mm tool is cutting slightly too much material, so I set its diameter to 6.05mm for the other parts.

An aluminium part

Yesterday, after drilling the holes for Part 0009 and making a couple of other small Delrin parts, I made this aluminum ( HE30 ) part for my friend Maaten. There was a mistake on the other side where a profile offset, for a counterbore, failed on HeeksCNC and I didn't realize. This caused the roughing passes to only have lead on and lead off moves, but no profile. The finishing pass, at full depth of 6.5mm was calculated OK, so when it machined the finishing pass, it was almost too much for it and the circular hole wasn't very round.
On the side we can see in the picture, the slots were mostly too wide, because the rough pocketing ( done with 0.1mm extra clearance at the sides ) was done in a "conventional" style, where the path goes clockwise, which caused it to take off too much material. I need to be able to specify "climb" or "conventional" for pocketing aswell as profiling.

Part 0009 done

I have done these. There were 8 of them to make. My Z travel was not enough to drill them with the drill, which needed an extra chuck, so I drilled them to 3mm deep with my little slot drill, which fitted in the collet, and then drilled them through on Dad's pillar drill.
This is all of the Delrin parts done, for this customer.

Mach 2010

I am here at Mach 2010, telling people about HeeksCNC software. I was thinking that Machine Tool manufacturers might be interested, but they mostly already have ties to commercial CAD/CAM software vendors. I spoke to Ian Walton from Cranfield University. I might help him make some software for his welding machine.

Parts 0010 and 0011

2 of each. 0011 was similar to 0010, so I only had to write a couple of operations again.

Part 0010

This part requires cutting on almost every side. The way the depth of cut works for pocketing is different to profiling in HeeksCNC. I must make them work the same.
For example the profile operation would have done this with depths of cut ( 5.125, 5.125, 5.125, 5.125 ), but the pocket operation used depths ( 5, 5, 5, 5, 0.5 )

Part 0007 finished

I have made the other copy of this part.
I think there are issues with hole depths, because I made this part 10.3mm thick ( to be sanded down to size ), but then I assumed that that it was 10mm thick for some of the holes.
This should mean that some of the holes are 0.2mm to 0.3mm too shallow.
I'll come back and have a look at these later.

Part 0007 1 done

I finished one of these parts. Now I must make another one. There are various things I am not happy about with this one. Having to cut it in at least 4 different setups has made it difficult to plan the clamping. In the top picture, I have cut the wood so that there is a post for one of the holes at the top right and an island for most of the big circle hole. This was not clamped ideally and you can see in the 3rd picture how the profile doesn't match up.
In the 4th picture, you can see where I made a programming error for one of the holes ( I had to program it separately from the others because of some geometry error I don't understand yet ). I accidentally typed the final depth in to the rapid-to height. This highlights the need for my software to warn me if the rapid-to height is below the start depth. In my next version of the software, the rapid-to height will be a relative distance above, instead of an absolute z height.