Haas Lathe Non Monotonous error

chevelless502 · Dec 14, 2017

We are having an issue with getting a Non Monotonous error with the following program. Can anyone shed some light on it as to what can be wrong?

T202
G50 S2000
G97 S700 M03
G96 S500 M08
G00 G54 X1.65 Z0.1

(Major spindle profile)
G71 G54 P103 Q104 D0.025 U0.02 W0.004 F0.01

N103 G00 X0.5
G01 X0.625 Z-0.063
G01 z-0.933
G02 X0.705 Z-0.974 R0.09
G01 X1.106
G01 X1.248 Z-1.099
G01 Z-2.938
G02 X1.312 Z-2.969 R0.031
G01 X1.5
G01 X1.625 Z-3.031
G01 Z-4.469

N104 X1.625
G70 P103 Q104

Thanks in advance

kenton · Dec 14, 2017

If I remember correctly Non Monotonous errors are usually in relation to radius moves so I would check those first.

bassbrawls · Dec 14, 2017

Try this:

N104 X1.65

Booze Daily · Dec 14, 2017

N103 G00 X0.5
G01 X0.625 Z-0.063
G01 z-0.933
G02 X0.705 Z-0.974 R0.09
G01 X1.106
G01 X1.248 Z-1.099
G01 Z-2.938
G02 X1.312 Z-2.969 R0.031
G01 X1.5
G01 X1.625 Z-3.031
G01 Z-4.469

N104 X1.625

These Z's don't work math wise.
Maybe you control is trying to calculate a bigger than 90 arc in which case Z would be non-monotonous.

vettedude · Dec 14, 2017

chevelless502 said:
We are having an issue with getting a Non

Thanks in advance

monotonic!

Troubleshoot your lathe G71 and G72 roughing cycles quickly – Haas Automation Tip of the Day - YouTube

guest · Dec 14, 2017

Looks like the R.09 should be R.04? Is that supposed to be a 90 degree arc?

chevelless502 · Dec 14, 2017

The operator just went in and switched the .090 to a .040 and we still get the same error.

doug925 · Dec 14, 2017

If this line "G02 X0.705 Z-0.974 R0.09" is not a full 90°, you might want to use a I & J instead of the (easy) R value.
I did not calculate/draw/back-plot the path, so forgive me if it IS a full 90° segment.

A Haas will give you about 0.001" of "fudge factor" on your coordinates, but will alarm out if more than.

Doug.

guest · Dec 14, 2017

chevelless502 said:
The operator just went in and switched the .090 to a .040 and we still get the same error.

Where in the program do you get the error? The numbers are off by .001", I wouldn't expect that to generate the error but you can change the Z-.933 to Z-.934. Also the G2 X1.312 can be X1.310 (1.248+.062).

You can change the R's to I's, leave the numbers and signs alone.

edit to add: also as brassbrawls noted- you should make the X position in the Q block X1.65 (same as the canned cycle start position).

angelw · Dec 14, 2017

chevelless502 said:
The operator just went in and switched the .090 to a .040 and we still get the same error.

Hello chevelless502,
Although the R0.09 would have been a mistake if a 90deg arc was required, the trajectory for a 0.09 radius will not give you the error that's being raised. Using the same Start and End point and a 0.04 radius is more likely to raise this error.

With your current program, its more likely that the error is with the 0.031 radius. Using your current arc Start and End points will result is a very slight movement in a Z+ direction at the end of the arc. Try the following to see if it works for you.

G01 Z-2.9380
G02 X1.3100 Z-2.9690 R0.0310

instead of

G01 Z-2.9380
G02 X1.312 Z-2.969 R0.031

X1.312 will result in a 91.878deg arc sector.

Also, I would do as bassbrawls suggested and use X1.65 in your P referenced block N104.

Regards,

Bill

chevelless502 · Dec 14, 2017

guest said:
Where in the program do you get the error? The numbers are off by .001", I wouldn't expect that to generate the error but you can change the Z-.933 to Z-.934. Also the G2 X1.312 can be X1.310 (1.248+.062).

You can change the R's to I's, leave the numbers and signs alone.

edit to add: also as brassbrawls noted- you should make the X position in the Q block X1.65 (same as the canned cycle start position).

That fixed it just by changing those two dimensions. Can you explain to us what brought you to that suggestion? My operator would like to know so he doesn't have this issue again.
Thank you for the help.

guest · Dec 14, 2017

chevelless502 said:
That fixed it just by changing those two dimensions. Can you explain to us what brought you to that suggestion?

I was assuming you wanted a 90 degree arc. So taking the start position of the G2, subtract the radius value from the Z position and add double the radius value to the X position. Those are the X and Z end positions of the 90 degree arc.

Your numbers were off by .001" and .002" respectively. That apparently was enough for the control to throw the error.

angelw · Dec 15, 2017

guest said:
I was assuming you wanted a 90 degree arc. So taking the start position of the G2, subtract the radius value from the Z position and add double the radius value to the X position. Those are the X and Z end positions of the 90 degree arc.

Your numbers were off by .001" and .002" respectively. That apparently was enough for the control to throw the error.

Hello jancollc,

Although the OP probably wanted a 90 deg arc, it still doesn't explain why a Non-monotonous alarm was raised when he had specified a 0.09 Radius. The R format is forgiving with regards to incorrect Start/End points, or Radius being specified. Forgiving in that no alarm is raised provided its geometrically possible to fit a given radius through the two given points, but not so forgiving in that the radius cut is not correct. If its geometrically possible, the control simply calculates an Arc centre based on the data provided.

Following is a picture of the layout of the OP's first radius. (R0.09)

Clearly there is no Non-monotonous move.

Further downstream in the following code, the arc sector cut is 91.878degs, with the trajectory for the radius moving in a Z+ direction slightly, starting at X1.310.

G01 Z-2.938
G02 X1.312 Z-2.969 R0.031

Regards,

Bill

chevelless502 · Dec 18, 2017

guest said:
I was assuming you wanted a 90 degree arc. So taking the start position of the G2, subtract the radius value from the Z position and add double the radius value to the X position. Those are the X and Z end positions of the 90 degree arc.

Your numbers were off by .001" and .002" respectively. That apparently was enough for the control to throw the error.

Can you tell me how you made that math work out? We cant seem to get the numbers to work out by doing that subtraction and addition. If you subtract the radius value from the Z-.974 you get Z-.884 and then add double the radius to the X .705 number you get X.885. Would those be the numbers we should be putting in as those values instead of the X.705 and Z-.974 then?

Sorry for the novice questions on this but we are new to it all and still learning.

guest · Dec 18, 2017

chevelless502 said:
Can you tell me how you made that math work out? We cant seem to get the numbers to work out by doing that subtraction and addition. If you subtract the radius value from the Z-.974 you get Z-.884 and then add double the radius to the X .705 number you get X.885. Would those be the numbers we should be putting in as those values instead of the X.705 and Z-.974 then?

No, you are using the end point of the arc- use the start point.

You are starting at X.625 Z-0.934. You want to calculate the end point of the arc to put in the G2 line.

For a R.04:

Add .080 to .625, you get the endpoint of the arc X.705
Subtract .04 from -.934, your endpoint is Z-.974

You are doubling the radius in X because you are programming a diameter.

Make sense?

Read again what Bill said- the alarm was caused by the second radius, which was commanding an arc greater than 90 degrees. The Z axis was being directed to reverse direction at the very end of the arc, that was the "non-monotonous" move.

Search

Largest Manufacturing Technology Community on the Web

Search

Haas Lathe Non Monotonous error

chevelless502

Plastic

kenton

Stainless

bassbrawls

Aluminum

Booze Daily

Titanium

vettedude

Stainless

guest

Guest

chevelless502

Plastic

doug925

Titanium

guest

Guest

angelw

Diamond

chevelless502

Plastic

guest

Guest

angelw

Diamond

chevelless502

Plastic

guest

Guest

Similar threads