First Aluminium cut

[JAZZCNC]

Which do you call the X axis.? one with twin screws or single.?

If it's the twin screw then this could be resonance from the long extension of the Z axis or tool deflection.? I get this on my machine when I'm pushing it too hard and too deep with large Z extension, thou I'm talking 3mm+ Doc in ALI.!

There are ways round this.

Lift the work closer to the spindle and keep the Z extension small as pos.
Keep the tool extension out of collet short as pos.

Take deeper slower cuts.!! . . Yep sounds crazy I know but there's more of the tool engaged so supported more. Try 1.5mm @ 800-1000mm/min 17,000rpm
Use a slower full depth finish pass with a small 0.1-0.2 stepover.
Try and clear the chips as much as possible, lube stops sticking but also clogs the slot and makes the chips stick which then get recut. This at best the gives a poor finish and if extreme can cause tool deflection and overheat then breakage. You can tell if recuts a problem because there'll be little random dents on the surface, not like what you have which is a nice wave rib thats why I think it's resonance from deflection, tool or Z axis.?

I've found the best solution is constant low pressure air clearing the chips with the odd shot of coolant to help with stickage. Just keeping the slot clear with the odd blast of air works ok and better than just coolant but for best affect the air needs to be constant so all chips are gone. ( Gets bloody messy, you'll have chips darn ye kegs in crack your arse every where.!! Get the Sudocream ready.:rofl:)

Personaly I'd just back off the feed, up the Doc and try again and clear the chips as much possible. If you need good finish then use a full depth finish pass.

Edit: Looking at the pics again, it looks like you have cut the chamfer on the outer profile line.? Try using an offset so the centre of the V is not on the line. This will get rid of that little step you have.
Some times the software will have chamfer tool path and in it there'll be an option to set the offset and it will calculate the rest to give you the correct depth for the chamfer length you need.
If not then when you offset you'll lose a bit of chamfer length so just cut a little deeper to regain the lost length.