Machining Holes Finish Cut

[MR-CNC]

Hi,
I was using Aspire 9 to produce a finish cut in two holes on a box lid and wondered why the spiral cut were not a continuous line.
Refer my attachments below in Aspire and the resultant G-Code plus output visual.
I had not seen this issue on previous versions of Aspire.
The STL shape was made with a tolerance of .001mm
And the holes a round.
Regards,
Mauri.

[MR-CNC]

Hi,
This time I only used Aspire to make the same example and cut, but still ended up with a similar end result.
Aspire files below.
Regards,
Mauri.

[jimwill2]

Are the holes flat on the bottom? I would not do a 3d of the holes if you can do the same thing with pocket toolpaths in 2d. It would be much quicker. I believe when you make a pocket with 3d the circles have rough edges because you are cutting the pixals instead of the lines. That is why you are getting strange sides to the pockets. I could be wrong.

[ger21]

.stl files are made up of multiple triangular faces. There are no "holes", circles, or arcs in .stl files.
If you want round holes and pockets, draw round vectors and use those for your toolpaths.

[Adrian]

To give you an idea of the difference doing it as pockets will not only be far more accurate it will also machine around 30 times faster...

[rscrawford]

Finish tool paths should be used as a last resort, when a 2D cut is not possible. It is the least efficient tool path possible.

The reason you are getting those jumps in the tool path is because a 3D shape in Aspire is not a mathematical formula shape. It is made from 3D pixels (voxels). This means that a circle is not actually a circle, but a shape with a jagged edge as if it were made from tiny lego blocks. So the tool path is simply following those jagged edges.

If you cut a 2D pocket tool path, you will be using arcs, which will give you a perfect circle in your tool path.

[MR-CNC]

jimwill2/jer21,
The Aspire version only is perfectly flat and round as it is made in Aspire only "no STL", even STL at .001mm would make no difference as both show the same result.
adrian/rscrawford,
Thank you, a logical answer.
Your answer provides the correct result, however it requires 2 toolpaths one for the bottom hole, then another for the top hole and to make the cutting time less I have to restrict the top hole from cutting air.
I would use this method to do the whole cutting process and make the last cut for the bottom a smaller depth, this would then be better than 3D roughing and 3D finishing.
Also to prevent any edge chipping I will make a final profile small cut around the edge.
Thanks,
Regards,
Mauri.

[MR-CNC]

Hi,
If I do the Top hole pocket first, then the bottom hole pocket all is good no wasted time and it is fast.
Regards,
Mauri.

[Olle]

jimwill2/jer21,
The Aspire version only is perfectly flat and round as it is made in Aspire only "no STL", even STL at .001mm would make no difference as both show the same result.
adrian/rscrawford,
Thank you, a logical answer.
Your answer provides the correct result, however it requires 2 toolpaths one for the bottom hole, then another for the top hole and to make the cutting time less I have to restrict the top hole from cutting air.
I would use this method to do the whole cutting process and make the last cut for the bottom a smaller depth, this would then be better than 3D roughing and 3D finishing.
Also to prevent any edge chipping I will make a final profile small cut around the edge.
Thanks,
Regards,
Mauri.

To reduce chipping and "fuzz" I would cut the deep hole first, then the shallow one. I assume the comment about "cutting air" refers to the smaller area that has already been removed when you make the deep cut, and all you have to do is to set the inner circle as a border for the upper cut. Even better: Draw a "helper circle" that's somewhat smaller, so the cut overlaps a bit.