[mmurray70]

Hi Tom,

Wondering if there might be any way to improve the cutter comp errors in Kmotioncnc? Seems to be an issue with internal sharp corners. I've learned to deal with this one most times.

Trying to do a small o ring groove here today, i have a nice lead in and lead out, no sharp corners, yet it still errors out. I am ramping down in a helix but im pretty sure i have done this before and it worked? Is the helix causing the problem? This is just doing a wear comp of a few thou, not offsetting the width of tool or anything. Thanks.

Mark

[Need TECH Help!]

Hi murray,
Sounds like a issue i had before, had to change the comp entry style to Fanuc. Are you using the Fanuc style comp in your Set up file?
https://www.dynomotion.com/wiki/inde...xample_G41/G42
Troy

[mmurray70]

No, I had no idea about this. This sounds like just what I need. I'll try changing it after i finish this job. Dont really want to risk damaging these parts. So i just copy this line: comp_entry_style FANUC_COMP_ENTRY_STYLE EMC_COMP_ENTRY_STYLE to the setup file? Does it matter where I put it?

Anything to watch out for with this? Why is this not the default setting?

[Need TECH Help!]

Here is my entire set up file as an example.

Attribute				Value		Other Possible Values

axis_offset_x			0.0			any real number
axis_offset_y			0.0			any real number
axis_offset_z			0.0			any real number
block_delete			ON			OFF
current_x				0.0			any real number
current_y				0.0			any real number
current_z				0.0			any real number
cutter_radius_comp		OFF			LEFT, RIGHT
comp_entry_style        FANUC_COMP_ENTRY_STYLE
cycle_r					0.0			any real number
cycle_z					0.0			any real number not less than cycle_r
distance_mode			ABSOLUTE	INCREMENTAL
feed_mode				PER_MINUTE	INVERSE_TIME
feed_rate				5.0			any positive real number
flood					OFF			ON
length_units			INCHES		MILLIMETERS
mist					OFF			ON
motion_mode				80			0,1,2,3,81,82,83,84,85,86,97,88,89
plane					XY			YZ, ZX
slot_for_length_offset	1			any unsigned integer less than 69
slot_for_radius_comp	1			any unsigned integer less than 69
slot_in_use				1			any unsigned integer less than 69
slot_selected			1			any unsigned integer less than 69
speed_feed_mode			INDEPENDENT SYNCHED
spindle_speed			1000.0		any non-negative real number
spindle_turning			STOPPED		CLOCKWISE, COUNTERCLOCKWISE
tool_length_offset		0.0			any non-negative real number
traverse_rate			199.0		any positive real number

I dont think it was known about till a few years ago when i brought it up. If i remember right the EMC setup is on the side of caution. Been currently running the Fanuc style on a couple of mills including my own and only issue i have ever had is sometimes KMCNC does not like the way Fusion outputs it and gives the same gouge pop up.

[mmurray70]

I tried adding that line, but still get the same error. here is my file:

Attribute				Value		Other Possible Values

block_delete			ON			OFF
current_x				0.0			any real number
current_y				0.0			any real number
current_z				0.0			any real number
cutter_radius_comp		OFF			LEFT, RIGHT
comp_entry_style        FANUC_COMP_ENTRY_STYLE
cycle_r					0.0			any real number
cycle_z					0.0			any real number not less than cycle_r
distance_mode			ABSOLUTE	INCREMENTAL
feed_mode				PER_MINUTE	INVERSE_TIME
feed_rate				5.0			any positive real number
flood					OFF			ON
length_units			INCHES MILLIMETERS
mist					OFF			ON
motion_mode				80			0,1,2,3,81,82,83,84,85,86,97,88,89
plane					XY			YZ, ZX
slot_for_length_offset	1			any unsigned integer less than 69
slot_for_radius_comp	1			any unsigned integer less than 69
slot_in_use				1			any unsigned integer less than 69
slot_selected			1			any unsigned integer less than 69
speed_feed_mode			INDEPENDENT SYNCHED
spindle_speed			1000.0		any non-negative real number
spindle_turning			STOPPED		CLOCKWISE, COUNTERCLOCKWISE
tool_length_offset		0.0			any non-negative real number
traverse_rate			199.0		any positive real number

Any other ideas?

[mmurray70]

Did a little more testing. I can do 2d contours with a helix lead in no problem. When I try to ramp in with a helix it will let me do the outside of the groove, but not the inside?? Same size/shape lead in on both.

Changing the code to arcs instead of linearizing the helix seems to work for this situation.

[TomKerekes]

Hi Murray,

I've been trying to find a solution/workaround.

When I try to ramp in with a helix it will let me do the outside of the groove, but not the inside?? Same size/shape lead in on both.

That makes sense. Imagine a polygon like an octagon. A cutter can go around the outside and cut a perfect polygon, but can't go around the inside without gouging.

Changing the code to arcs instead of linearizing the helix seems to work for this situation.

Yes a cutter can go around the inside or outside of a circle without gouging.


I was thinking a workaround would be change the CAD to make the "polygon" slightly undersized. Then changing the compensation could be used to make it the correct size. I think this would work but the second "lead in" forms a path like an 'S". So there isn't a side where one side or the other doesn't gouge. If the lead in were changed or used arcs then I think it would run.

Note the wiki here describes the "lead in" types.

[mmurray70]

Ok I think I understand now. So because it was linearized it cant work with all the tiny sharp corners when compensating inwards. Makes sense. I was using a negative wear comp with this, just tried a positive value and got the same error on the first curve. And your right, the second curve gives an error with positive and negative values because it has the "S" in it creating a problem either way. This "S" problem explains to me why this would sometimes work, and not other times.

Well now that I know whats happening I adjusted my software to output arcs and hopefully this will do it for me in most cases. Still might have the occasional part with a sharp corner that gives me an error, but ill just have to remember to put a tiny rad there. Would be handy to have a proper fix maybe in a future version , most controllers would have no problem with this.

Should I stick with the Fanuc entry or change it back to the way it was?

[Need TECH Help!]

I ran into more comp gouge error issues when doing small inside shapes when using emc entry. Tested same gcodes on several different VMCs that never had an issue, so i just kept using the Fanuc entry in KMCNC.
Troy