New Machine Build- My lithophane with EMC2 image to gcode

[ktchk]

Hi

I am using EMC2 image to gcode to produce my first lithophane like the following


Every thing works fine with my Chinese made machine.

Thanks

K.T.Chan

[fritzgutten]

what material are you using?

[ktchk]

I got the 100x100x5mm corian (dupont) form their sale person. good for cutting.
I did tried with plastic cutting broad for kitchen.(cheap)
white arcalic also can do but the transparency (that is the white part of the picture) is not as good.

[stiyke]

Hi
Could you tell me the settings u used on the image to gcode in emc2?? i have tried twice and all it does is to draw lines. Do i have to convert the image to bump maps first before feeding it to emc2?? what type of cutting tool did you use v or ball nose or flat nose?? I appreciate your reply thanks.

[ktchk]

Hi Stikyke

The setup for image to gcode is as following:
invert image yes
normalize yes
extend image border none
tolerance .01 (the machine limit)
pixel size .25 ( the size of engrave in mm / pixels total ) most important cause most error
feedrate 2000
plunge feed rate 2000
spindle speed 2000
scan pattern rows
scan direction alternating
depth 4 mm ( the engrave depth)
step over 2
tool dia 1mm
safety height 0
tool type flat end
roughing offset 1
roughing depth per pass 2

Hope that helps
post if it works.

Regards

[stiyke]

Hello ktchk,

I tried your settings, it took me long to reply cause i had small issues i needed to sort in the machine. Its home built, and i cant find parts readily here am in Nigeria.
When i tried using ur setting i got same result it only cuts in xy on same depth. the z axis remains stationary most of the time. As you can see from those white material i had there in the pic.
Do you know what could be causing it?? i dont know why the Z axis doesnt move most of the time it cuts.
thanks
Iyke

[stiyke]

Sorry here is the pic of the machine and the sheet it cut

[ktchk]

Hi
The Z movement depended on the image black and white and the setting of "normalize" set to yes, "depth" set to thickness of material minus 1mm, zero or home of z axis set to surface of material. Chick up and test again.

[stiyke]

Hi Ktchk,

i inspected the Gcode and i think its working, so i have to zero at about 1.5mm above the work. I did cut a 3d on wood and it was almost through but my tool burnt i have to get a means of evacuating the dust/chips maybe a vacuum or blower. I feel the machine is ok now i will cut more tomorrow but not so deep to avoid burning the tool again.

Thanks

[ktchk]

If you need, the "roughing" can let you cut in layers 1mm in one layer the "roughing offset" can set the layer does not touch the high points until the last layer.

EMC2 can also set the tool movement speed to slow down until tips can handle the cut.