Fault at the control over "020 tolerance of radius"

[Oppiz]

After switching over to X7, I'm having trouble with arcs. Just doing basic lead in/outs and circle pockets. I get the error at the control "020 tolerance of radius". I believe I'm using the same setting as I did in X6. I'm using wear comp. Any ideas?

[specv]

can you show us some code?

[TK-32™]

^ X2

[Oppiz]

%

O3333

N1 G00 G17 G20

N11 G40 G80

N1 T1 M06 ( 3/4 FLAT ENDMILL)

N11 (MAX - Z.25)

N21 (MIN - Z-.75)

N31 G00 G90 G54 X2. Y-2.25 S1023 M03

N41 Z.25 M08

N51 Z.1

N61 G01 Z-.375 F6.42

N71 X2.1005 F9.41

N81 G41 Y-2.3505

N91 G03 X2.2009 Y-2.25 I2.1005 J-2.25

N101 X2. Y-2.0491 I2. J-2.25

N111 X1.7991 Y-2.25 I2. J-2.25

N121 X2. Y-2.4509 I2. J-2.25

N131 X2.2009 Y-2.25 I2. J-2.25

N141 X2.1005 Y-2.1495 I2.1005 J-2.25

N151 G01 G40 Y-2.25

N161 X2.

N171 G00 Z.25

N181 Z-.275

N191 G01 Z-.75 F6.42

N201 X2.1005 F9.41

N211 G41 Y-2.3505

N221 G03 X2.2009 Y-2.25 I2.1005 J-2.25

N231 X2. Y-2.0491 I2. J-2.25

N241 X1.7991 Y-2.25 I2. J-2.25

N251 X2. Y-2.4509 I2. J-2.25

N261 X2.2009 Y-2.25 I2. J-2.25

N271 X2.1005 Y-2.1495 I2.1005 J-2.25

N281 G01 G40 Y-2.25

N291 X2.

N301 X2.1055

N311 G41 Y-2.3555

N321 G03 X2.2109 Y-2.25 I2.1055 J-2.25

N331 X2. Y-2.0391 I2. J-2.25

N341 X1.7891 Y-2.25 I2. J-2.25

N351 X2. Y-2.4609 I2. J-2.25

N361 X2.2109 Y-2.25 I2. J-2.25

N371 X2.1055 Y-2.1445 I2.1055 J-2.25

N381 G01 G40 Y-2.25

N391 X2.

N401 G00 Z-.125 M09

N411 G28 Z0.

N421 G28 Y0.

N431 G90

N441 M30

[specv]

what line does it alarm on?

[TK-32™]

The code looks good. You don't have a crazy offset on the cutter comp do you?

 

What control is giving you this problem?

[Brando]

could be you need to force x and y output on the g41 and g40 line, or do a strait line move after the g41 line, before the g03

[Oppiz]

what line does it alarm on?

 

 

N81 G41 Y-2.3505

[Oppiz]

The code looks good. You don't have a crazy offset on the cutter comp do you?

 

What control is giving you this problem?

 

Fanuc 18I

 

cutter comp .0015

[TK-32™]

Does your control require a D value in the G41 line like FANUCs?

[Oppiz]

Does your control require a D value in the G41 line like FANUCs?

 

nope

[TK-32™]

can you post a similar program with X6 and compare the two codes?

[specv]

Our fanucs require a D value for comp otherwise it does not know what offset to use.

[Rstewart]

Our fanucs require a D value for comp otherwise it does not know what offset to use.

 

 

^^^^

Yes

[Oppiz]

I've been doing some more testing. What settings do I need to change? This is a circle pocket 1.5 DIA with a 1/2 em

 

 

 

THIS DOESN'T RUN

 

O0000 (TESTNEW)

(T4 | 1/2 FLAT ENDMILL | H0 | D0 | D0.5000" | | CONTOUR....)

N4 G00 G17 G20

N14 G40 G80

N4 T4 M06 ( 1/2 FLAT ENDMILL)

N14 (MAX - Z.25)

N24 (MIN - Z-.75)

N34 G00 G90 G54 X0. Y0. S1200 M03

N44 Z.25 M08

N54 Z.1

N64 G01 Z-.3725 F6.42

N74 G41 X.25 Y.25 F12.

N84 G03 X0. Y.5 I0. J.25

N94 X-.5 Y0. I0. J0.

N104 X0. Y-.5 I0. J0.

N114 X.5 Y0. I0. J0.

N124 X0. Y.5 I0. J0.

N134 X-.25 Y.25 I0. J.25

N144 G01 G40 X0. Y0.

N154 G00 Z.25

N164 Z-.2725

N174 G01 Z-.745 F6.42

N184 G41 X.25 Y.25 F12.

N194 G03 X0. Y.5 I0. J.25

N204 X-.5 Y0. I0. J0.

N214 X0. Y-.5 I0. J0.

N224 X.5 Y0. I0. J0.

N234 X0. Y.5 I0. J0.

N244 X-.25 Y.25 I0. J.25

N254 G01 G40 X0. Y0.

N264 G00 Z-.1225

N274 Z-.645

N284 G01 Z-.75 F6.42

N294 G41 X.25 Y.25 F12.

N304 G03 X0. Y.5 I0. J.25

N314 X-.5 Y0. I0. J0.

N324 X0. Y-.5 I0. J0.

N334 X.5 Y0. I0. J0.

N344 X0. Y.5 I0. J0.

N354 X-.25 Y.25 I0. J.25

N364 G01 G40 X0. Y0.

N374 G00 Z-.495 M09

N384 G28 Z0.

N394 G28 Y0.

N404 G90

N414 M30

%

______________________________________

 

 

THIS DOES RUN

 

O0000 (TESTOLD)

(T4 | 1/2 FLAT ENDMILL | H0 | D0 | D0.5000" | | CONTOUR....)

G00 G17 G20

G40 G80

N4 T4 M06 ( 1/2 FLAT ENDMILL)

(MAX - Z.25)

(MIN - Z-.75)

G00 G90 G54 X0. Y0. S1200 M03

Z.25 M08

Z.1

G01 Z-.3725 F6.42

G41 X.25 Y.25 F12.

G03 X0. Y.5 I-.25 J0.

Y-.5 I0. J-.5

Y.5 I0. J.5

X-.25 Y.25 I0. J-.25

G01 G40 X0. Y0.

G00 Z.25

Z-.2725

G01 Z-.745 F6.42

G41 X.25 Y.25 F12.

G03 X0. Y.5 I-.25 J0.

Y-.5 I0. J-.5

Y.5 I0. J.5

X-.25 Y.25 I0. J-.25

G01 G40 X0. Y0.

G00 Z-.1225

Z-.645

G01 Z-.75 F6.42

G41 X.25 Y.25 F12.

G03 X0. Y.5 I-.25 J0.

Y-.5 I0. J-.5

Y.5 I0. J.5

X-.25 Y.25 I0. J-.25

G01 G40 X0. Y0.

G00 Z-.495 M09

G28 Z0.

G28 Y0.

G90

M30

%

[Brando]

it seems the i or j in the second program has a - sign which is correct, and the first does not

[TK-32™]

If the one that runs is from X6 check in in your control configuration that you have both values for arcs the same from your X6 to X7 control config.

Here's how ours looks like:

[specv]

Check the arc settings in the control def. it looks like your settings should be set this way.

[Alien]

After switching over to X7, I'm having trouble with arcs. Just doing basic lead in/outs and circle pockets. I get the error at the control "020 tolerance of radius". I believe I'm using the same setting as I did in X6. I'm using wear comp. Any ideas?

 

Hi,

you can find answer here http://cnc-professional-forum.com/threads/2206-020-over-tolerance-of-radius

Good luck!

Sincerely,

Michael.

[Guest MTB Technical Services]

Check Parameter No. 3410 on the control.

 

In circular interpolation (G02 or G03), difference of the distance between the start point and the center of an arc

and that between the end point and the center of the arc exceeded the value specified in parameter No. 3410

 

Some observations.

The new program is breaking arcs at the quadrants and the old one is not.

 

Also, you aren't calling a tool length offset or a tool radius offset.

If you don't specify the D address for your CRC offset, the system will use the last modal value if one exists.

[Oppiz]

I got it. It was the arc settings that were causing the problems. The reason this happened was my post weren't updated correctly. Thank you everyone for the help!

[mike93]

with only a .250 lead in with a .500 cutter you can only run 0 or a neg value in your wear comp i think with a .0015 wear you needa .2515 radius or more

[Guest MTB Technical Services]

with only a .250 lead in with a .500 cutter you can only run 0 or a neg value in your wear comp i think with a .0015 wear you needa .2515 radius or more

 

Wrong.

As long as the total comp amount fits within the radius to be cut there isn't an issue with CRC.

You are assuming he's entering the entire tool radius in the offset register.

That would mean he's programming for part geometry values. VERY BAD IDEA.

 

Anyone not using wear comp in Mastercam is asking for scrap on a Fanuc controlled Mill.

ALWAYS program for the center of the tool when using CRC (Mastercam Wear Comp).

This way all CRC values are always wear values at the control and should start at 0 in theory.

If reground mills are used you simply enter the radial difference in the register.

Programing part geometry values is a recipe for scrap.

Forget a small wear offset and you can probably save the part.

Forget a complete radial offset and the part is scrap.

 

The Toolpath he programmed has a linear lead-in and a ramp-in radius.

Plenty of room for a wear offset.

 

The real issue was the output was using absolute arc centers in the new program.

Take note of the I0.0, J0.0 in the new program.

 

Fanuc uses incremental I,J,K .

That is, the distance from the start point to the center of the arc is an incremental value.

 

You can never have I &J both be zero on a Fanuc.

[Newbeeee™]

 

Anyone not using wear comp in Mastercam is asking for scrap on a Fanuc controlled Mill.

Fully agree with what you said, but unfortunately we're machine comp here. I wish we understood wear when we started the business but there's bucket loads of progs now and I can see it would be a nightmare to change.

The only saving grace is that our offset is entered into the control via G10, so it's saved in the prog. This stops the forgetting bit.