Doosan Mill Fanuc Control- G41 Help

David.Kemmer · May 8, 2019

Hello all,

Quick question regarding how my Doosan mill is reacting when I make a move to turn on G41 cutter comp.

I'm simply staging the cutting 2x cutter diameter from the first point in X, and then making a single axis move to the first point to turn the compensation on.

Example: (X0. Y0. is the part center)

G43 H20 Z.1
G0 X2. Y0.
G1 Z-.5 F20.
G41 D20 X1. F15.

As you can see I'm only making a move in the X axis to turn on the comp, but the machine physically compensates the Y axis as well so my Y tangent point is below (negative) from Y0. Why does this happen when I don't specify a Y move in the G41 line? It's seems that the same code on my HAAS machines will only move the X axis while turning on the comp unless a Y move is specified. I've also tried staging the Y axis above and below the part center line by the cutter diameter, and I always seem to end up below Y0. once the G41 line is complete. Any help is greatly appreciated!

Tichy · May 8, 2019

Sounds a bit odd. I run a Doosan mill too but... never noticed this behavior? Will check. What are the rows of code after what you posted?

Still: If your cutter radius is 1 and you go distance 1, you don't move at all. IIRC you need to actually move to turn on radius compensation correctly (preferrably distance of mill diameter or more) but I may just be confused.

Note, you can turn on radius compensation this way and then do Z- on next line with no problem. You can also disengage with G40 Z* (quick n dirty.)

David.Kemmer · May 9, 2019

Tichy,

I tried turning it on before the Z move, after the Z, staged the Y positive & negative one radius length; nothing seems to work. The next several lines of code after my example above are calculating the next X & Y point of the polygon being milled. I simplified the aforementioned example, but I get the same problem when I run the exact code. The true program is as follows:

#110=#24+ COS [#105]*#18
#111=#25- SIN [#105]*#18
G90 G0 X[#110+#20*1.5]
G1 Z-#131 F20.
G41 D#500 G1 X#110 Y#111 F#9
#104=#104+1
#105=#105+#103

N1 IF [#104GT#19 ]GOTO100
#110=#24+ COS [#105]*#18
#111=#25- SIN [#105]*#18
G1 X#110 Y#111 F#9
#104=#104+1
#105=#105+#103

I'm curious about maybe a "read-ahead" issue or I guess I'm really at a loss right now.

Tichy · May 9, 2019

David,

Polygon macro, cool

Made a similar thing in school but I just G16'd it.

In the aforementioned code I would suggest that the tool will move in Y because it will assume a position at a 90' angle to the line it's about to cut, i.e. if the cut is at 220' then the mill will position itself at 310' at a distance of D. Yes, it's look-ahead.

DouglasJRizzo · May 9, 2019

Normal. Rapid position the Y below where it should be and the X around 2X away from the part. Engage G41 in X to a distance that's still not touching, then Y up to correct and go to work. I have the training manuals if you need.

angelw · May 9, 2019

David.Kemmer said:
Tichy,

I tried turning it on before the Z move, after the Z, staged the Y positive & negative one radius length; nothing seems to work. The next several lines of code after my example above are calculating the next X & Y point of the polygon being milled. I simplified the aforementioned example, but I get the same problem when I run the exact code. The true program is as follows:

#110=#24+ COS [#105]*#18
#111=#25- SIN [#105]*#18
G90 G0 X[#110+#20*1.5]
G1 Z-#131 F20.
G41 D#500 G1 X#110 Y#111 F#9
#104=#104+1
#105=#105+#103

N1 IF [#104GT#19 ]GOTO100
#110=#24+ COS [#105]*#18
#111=#25- SIN [#105]*#18
G1 X#110 Y#111 F#9
#104=#104+1
#105=#105+#103

I'm curious about maybe a "read-ahead" issue or I guess I'm really at a loss right now.

Hello David,
Your Post shown above and your first Post, tell conflicting stories. In the above Post, your Tool Radius Comp Start Up Block has a move in two axes. Post the whole of the Macro and some typical values for the variables being used.

In the mean time, what setting do you have for parameter 5003.1?

Regards,

Bill

David.Kemmer · May 9, 2019

Tichy said:
David,

Polygon macro, cool Made a similar thing in school but I just G16'd it.

In the aforementioned code I would suggest that the tool will move in Y because it will assume a position at a 90' angle to the line it's about to cut, i.e. if the cut is at 220' then the mill will position itself at 310' at a distance of D. Yes, it's look-ahead.

I just found out that the machine I'm using is indeed equipped with the G16 command albeit the only one in the shop lol. :cheers:

I was practicing making a G65 macro to cut a polygon based on the # of sides and radius specified by the user. G16 will come in handy!

David.Kemmer · May 9, 2019

angelw said:
Hello David,
Your Post shown above and your first Post, tell conflicting stories. In the above Post, your Tool Radius Comp Start Up Block has a move in two axes. Post the whole of the Macro and some typical values for the variables being used.

In the mean time, what setting do you have for parameter 5003.1?

Regards,

Bill

You are correct, but the Y value in the comp line is the same value as the staging position (Y0). I have tried removing the Y position in the comp line, and the outcome is identical. The starting angle (#105) is 0, #18=.81, #24 & #25 (X & Y position)=0.

Parameter 5003.1 is set to 0. I looked into the Fanuc parameters, changed 5003.1 to a 1, and now the cutter comp works the way I want it to!! Thank you for turning me onto that parameter. :smitten:

Search

Largest Manufacturing Technology Community on the Web

Search

Doosan Mill Fanuc Control- G41 Help

David.Kemmer

Plastic

Tichy

Aluminum

David.Kemmer

Plastic

Tichy

Aluminum

DouglasJRizzo

Titanium

angelw

Diamond

David.Kemmer

Plastic

David.Kemmer

Plastic

Similar threads