Cutting a curved shape from a block of aluminum

[JAZZCNC]

Rufe0 he needs it concaved your code is convexed.

[phill05]

There you go 4x4 saved as a STL let me know

[Jonathan]

Rufe0 he needs it concaved your code is convexed.

Also, by programming a ball-nose tool to trace an arc, it will not cut the same path, unless the tool radius is zero! This is due to the way the contact point on the tool moves - my quick diagram should make it obvious:

[JAZZCNC]

Try it Old school and learn G-code from Master TP (terry parker).!!! https://www.machsupport.com/forum/in...?topic=24988.0

[Rufe0]

RE: JAZZCNC

It looks pretty concave to me, I guess if you had your machine set with the Z low at the top and high at the bottom then it would be, anyway it's a simple task to do file>replace the G2>G3 and vise versa.

RE: Jonathan

Yes I forgot to mention he would need a ball nose tool with radius less than 5 17/32.

You could do it longitudinally with a normal endmill but you'd be massively wearing the tooth corners out and it would take practically a million passes to get smooth.
The ideal way todo this would be with a fly cutter however you'd need a horizontal mill, unless you could fix the work piece vertically.

[Jonathan]

RE: Jonathan

Yes I forgot to mention he would need a ball nose tool with radius less than 5 17/32.

or equal to! But more seriously, that's not the point I was making - your code will be more accurate as the tool diameter tends to zero, so clearly you need to compensate the tool height as in my diagram.

I'm not sure that the code Jazz has linked to does this either?

[JAZZCNC]

RE: JAZZCNC

It looks pretty concave to me, I guess if you had your machine set with the Z low at the top and high at the bottom then it would be, anyway it's a simple task to do file>replace the G2>G3 and vise versa.

Hey!! Think you'll have to explain that one to me.? Only way that code would cut concave is if machine was upside down . . . But like you say to get it concave is easy fix but still not correct because like Jon points out there's no tool height Comp.

I'm not sure that the code Jazz has linked to does this either?

Think it does Jon because he's got tool dia in one of the params and does some maths with it but I haven't checked it so could be wrong.!! . . . Terry isn't a muppet so would have took the easy route I'm sure if not.?

[Jonathan]

Think it does Jon because he's got tool dia in one of the params and does some maths with it but I haven't checked it so could be wrong.!! . . . Terry isn't a muppet so would have took the easy route I'm sure if not.?

To cut the correct concave profile, you need to cut along a diameter which is the tool diameter subtracted from the diameter of the surface you wish to cut. Having looked more carefully, I can confirm that Terry has done this (the line #1000=[#1040-#1030]), so barring other errors, he is not a muppet, at least in this case.

I plotted a graph to demonstrate. The blue line represents the desired surface, red line is the toolpath (so an arc of radius [r_surface-r_tool]), and the red circles represent the tool. You can see it touches nicely at a tangent.



So, sorry Rufe0, but in Jazz's words, you apparently are a muppet!

[JAZZCNC]

So, sorry Rufe0, but in Jazz's words, you apparently are a muppet!

Ah ah you shit stirring little Geek I wasn't calling anyone a Muppet or having a go at Rufe0 so bugger off and twiddle some wires. .

[Rufe0]

Hey!! Think you'll have to explain that one to me.? Only way that code would cut concave is if machine was upside down . . . But like you say to get it concave is easy fix but still not correct because like Jon points out there's no tool height Comp.

Ah I think I've figured out the confusion, in mach 3 it's convex but I was using quick and dirty toolpath simulator. Tried it in a couple other simulators I had when you questioned it and they where all concave. I think it's the G18 XZ axis designation, in Mach3 the CW/CCW circular interpolation is in respect to the back elevation whereas everything else it's the front.