Fanuc alarm: 41 - INTERFERENCE IN CRC /NRC

[Anonymous]

Hi Guys, i was running a part and i was doing a circular hole and on the first few lines of code i got this error. i looked it up and says it has to do with the post. i wanted to know if anyone got this error before? and do i need to modify the post? 

Let me know, Eli 

  Fanuc alarm: 41 - INTERFERENCE IN CRC /NRC

CNC Machine Control Manufacturer

Fanuc

Control Model

16/18/21, 16i/18i/21i, 160i/180i/210i, 0/00/0-mate, 0i

41 - INTERFERENCE IN CRC /NRC

Alarm Description

Overcutting will occur in cutter compensation C. Two or more blocks are consecutively specified in which functions such as the auxiliary function and dwell functions are performed without movement in the cutter compensation mode. Modify the program. Overcutting will occur in tool nose radius compensation. Modify the program. Overcutting will occur in tool nose radius compensation.
Modify the program.

[patrik_stellgren]

Hi

Under your operations passes tab, check your wear offset. This is set to "In computer" by default, which means your tool compensation is calculated in the CAM software, hence requiring your tool radius / dia offset in your machine controller  to be set at 0. But this shouldn't produce any G41/42 in your code.

If you are using "Wear" instead, it will tell you the maximum allowed wear offset that can safely be used in the control.

I would try decreasing the value of your tool radius in the control and see if it helps

[Laurens-3DTechDraw]

---

@patrik_stellgren wrote:

Hi

Under your operations passes tab, check your wear offset. This is set to "In computer" by default, which means your tool compensation is calculated in the CAM software, hence requiring your tool radius / dia offset in your machine controller  to be set at 0. But this shouldn't produce any G41/42 in your code.

If you are using "Wear" instead, it will tell you the maximum allowed wear offset that can safely be used in the control.

I would try decreasing the value of your tool radius in the control and see if it helps

---

There is no need to have it set at 0 if you are using in Computer.

The machine doesn't do anything with it if you are using in computer.

[Anonymous]

Hi there, 

my problem is that when i set it to wear in computer it cuts the pocket .040" too short, when i tried to put wear i set the max to what is recommended and i put in my machine as wear in the tool -.001 just as a start but as soon as i do that i get those errors. 

my control is Fanuc 0i-mc VMC.

its weird i dont know what its doing it. i put a screen shot of the of the tool so you can take a look. 

Thanks, Eli. 

[Laurens-3DTechDraw]

---

@Anonymous wrote:

Hi there, 

my problem is that when i set it to wear in computer it cuts the pocket .040" too short, when i tried to put wear i set the max to what is recommended and i put in my machine as wear in the tool -.001 just as a start but as soon as i do that i get those errors. 

my control is Fanuc 0i-mc VMC.

its weird i dont know what its doing it. i put a screen shot of the of the tool so you can take a look. 

Thanks, Eli. 

---

Can you make a screenshot of the lead-in and out settings?

I think your lead-in length is too short.

[Anonymous]

here is a screen of the lead in lead out

[biester26]

I don't have a Fanuc simulator but I do have a Mitsubishi M70 simulator on my laptop and the code runs just fine.  This (I feel) is a control issue.  I would try disabling the horizontal and vertical radius lead ins and use a perpendicular linear lead-in to pick up the comp and increase the lead-in value to at least .100".  See if that will help.

[Anonymous]

ok i will try that tomorrow and see what happens.

Thank you for your help.

Eli.

[Anonymous]

ok i will try that tomorrow and see what happens.

Thank you for your help.

Eli.

[Anonymous]

Hello, 

i tried doing that and i am still getting the same error. if i dont use wear and i use computer i dont have the error. if i use wear in my control with g41 g42 g43 i get the errors. 

[biester26]

Can you tell me the year make and model of the machine you are trying to run this code on?  Which specific Fanuc control is on this machine?  Have you been successful before using wear comp on this control?

[Anonymous]

Hi there, 

i have 2 VMC they are made by Dhalih MCV-720 one is with Fanuc 18I-MB and the other is 0I-MC. the 0I has a 4th axis on it. 

if i program with a wear option i get the error code, i put in the machine in the tool wear a negative number such as -0.001 for example.

of i put 0 the machine ignores the g41 g42 g43

Let me know what do you think?

Eli.  

[patrik_stellgren]

Do you have both tool dia offset and wear offset in the fancy control?

If you do, have you set the tool diameter as well?

Patrik

[Anonymous]

in the control i have tool hight which is H in the program. everytool has a diameter data and D for wear.

its all in the control.  

[patrik_stellgren]

okay i think your  control uses  tool D + wear = total tool dia   for the g41/42 commands. But with wear you can ONLY enter wear offset.  so basically 0 +- wear...  change operation  wear to in control.   that will give you larger lead ins.   Or zero out the tool Dia in the control and only use wear if that works for your fanuc control.

Because now your lead in is insufficient to move over your tool..  

[patrik_stellgren]

need to correct myself,   it's not only about the lead ins, but  you can't cut a inside arc that is smaller than your tool radius which is why your controller errors out i guess. 

[Anonymous]

HI Patrik, 

im attaching the PDF part of my manual that has to do with the cutter comp. there's an issue and it has nothing to do with the wear if i call in the program g41 or g42 and the D in the machine is 0 it cancels the cutter comp automatically.  the machine reads two lines ahead in the code and if it sees two cutter comps it triggers an alarm. take a look and let me know what you think. im going to call Fanuc on monday and see what they say.

Thanks, Eli. 

[patrik_stellgren]

Okay, let's go down to basics.  Looking at your code

N60 G18 G02 X-1.961 Z-0.0415 I0.05
N65 G17
N70 G01 G41 X-1.936 D03

Your tool dia is .5"   tool radius is .250"  correct?

G41, cutte comp move is about  .025" inches?? ( distance between N60 and N70 blocks)  

How do you want the control to move your tool ( .250" ) in a distance of .025" I'm pretty sure EVERY control would error out on that.  So it's not your fanuc control.

That move needs to be at least .250" 

Now, I MIGHT be wrong but this is what works for me.

I use compensation type   WEAR       99% of time.  

WEAR already puts out a compensated tool path.   What does this mean?  It means HSM is creating a tool path that is already compensated, i.e. moved from the  desired tool path out by the radius of the tool..

So if it was to do a simple linear move from lets say     X0Y0  to X1Y0  with a .5" radius tool it would produce a Gcode of X0Y.5 to X1Y0.5 if it was to be compensated on the left side / climb cutting.

this means you CAN NOT have a tool radius in the control because then you are double compensating. Tool radius offset in control should be ZERO or the WEAR of the tool.  And HSM is clever enough to tell you what a safe value would be, (from your picture it would be 0.0125"  and as you can see your .250 is way larger.

now when i said you should use zero value, i don't mean D0, no it should be D03 as your program. but on your tool offset page offset 03 (d03) should be zero.  Now if your control doesn't  allow that, i don't know. then put in a small number like 0.001 and that should let you run your program.

If you DONT want to zero out all your offsets in the machine then I suggest you use compensation type "In Control"  this way HSM will put out non compensated tool path  and you need to program tool diameter and wear offsets at the control.

I hope this helps and isn't too confusing.

[biester26]

I am curious to see what the Monday phone call uncovers.  Have you run comp like this in this machine before?  Have you used a negative comp value with success prior to this program?