I was using a 4mm endmill in aluminium and the cutting tool was used for the trochoidal for the main cutting, but also the same tool used for drilling.
When it came to the drilling section the set depth of 0.5mm was ignored and did a full depth cut of 7mm, stalling my machine.
I had to re-program the CAM file to add another tool (same tool, different settings) just for drilling and set the depth to 0.5mm and ignored the tool change when it came up during the machining.
I was lucky that no damage was done to my machine or tool this time.
Image shows the original setting for the 4mm tool used.
I noticed this same behavior with trochoidal milling. I asked @christian-knuell about it in the main Estlcam 12 thread
061 has just been released and after testing the problem still exists
These drills are suppose to be in 0.5mm pecks
(No. 2 Drill machining: Drill 6)
G00 X71.256 Y33.209 Z5.000
G00 Z0.500
G01 Z-7.000 F400
G00 Z5.000
(No. 3 Drill machining: Drill 5)
G00 X87.487 Y33.221 Z5.000
G00 Z0.500
G01 Z-7.000 F400
G00 Z5.000
(No. 4 Drill machining: Drill 2)
G00 X78.828 Y53.029 Z5.000
G00 Z0.500
G01 Z-7.000 F400
G00 Z5.000
Hello,
please try the drill function again - It should now be OK with 12.062.
Christian
4 Likes
That is better, thanks Christian.
(No. 2 Drill machining: Drill 6)
G00 X71.256 Y33.209 Z5.000
G00 Z0.500
G01 Z-0.500 F400
G00 Z0.500
G00 Z0.000
G01 Z-1.000
G00 Z0.500
G00 Z-0.500
G01 Z-1.500
G00 Z0.500
G00 Z-1.000
G01 Z-2.000
G00 Z0.500
G00 Z-1.500
G01 Z-2.500
G00 Z0.500
G00 Z-2.000
G01 Z-3.000
G00 Z0.500
G00 Z-2.500
G01 Z-3.500
G00 Z0.500
G00 Z-3.000
G01 Z-4.000
G00 Z0.500
G00 Z-3.500
G01 Z-4.500
G00 Z0.500
G00 Z-4.000
G01 Z-5.000
G00 Z0.500
G00 Z-4.500
G01 Z-5.500
G00 Z0.500
G00 Z-5.000
G01 Z-6.000
G00 Z0.500
G00 Z-5.500
G01 Z-6.500
G00 Z0.500
G00 Z-6.000
G01 Z-7.000
G00 Z5.000
1 Like