Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Arc issue on Fanuc


Guest
 Share

Recommended Posts

OK, I am having a problem with a customer occasionally

 

It has come up with 2D paths HS paths, 3D paths, it will on occasion create a large loop that violates the geometry.

 

Arcs are set to break @ quadrants

 

The only thing to date that has worked is linear output

 

I thought I remembered a post about an issue with Fanuc and parameters for how it calculates arc endpoint needing to be tightened or changed but I cannot find it

Link to comment
Share on other sites
Guest MTB Technical Services

Parameter #3410 - Tolerance of arc radius

 

Change it from 10 to 100, or simply increase the value present.

It shouldn't take much.

 

You can also take a look at #3403.

Link to comment
Share on other sites

set to no rounding on the check end point

 

but changing parameters might be better as mtb said

 

I have ran into this before, why do some fanuc controls go around  wrong and some work right maybe its a random parameter generator?

 

if you plot the arcs out in the problem areas you will most likely  find out that thy do not connect with the start and end points.

Link to comment
Share on other sites

I have seen first hand on Mazak and Haas a case where arcs greater than 99.9 inches (110" in our case) cause the machine to go to never-never land (big loops).   We programmed it with Mastercam , Unigraphics, and manual g-code.  Arc endpoints were within .0001" from all 3 programming methods.  We then spent 7 months back and forth with Mazak both Chicago and Japan trying to diagnose the problem.. Mazak tried running our code on several different machines and all went to never-never land.  The bottom line according to Mazak Japan at the time (2007) was that the NC control just couldn't handle arcs larger than 99.9".  The solution was to linearize the large arcs.

  • Like 1
Link to comment
Share on other sites

No matter what I have tried, changing minimum arc size, limiting the size of arcs, the machine has gone to never, never land

 

He has his Machine/Fanuc guy going in on Monday, has has the parameter issue and they are going to try to diagnose.

 

In this case it is a Surface Finish Blend path machining a .02"R on a 3D surface, I Have done stuff like this 100 times if I have done it once

 

I did try to linearize but then of course it wouldn't fit into the machine memory.

 

So I will await the Monday powwow and work with them to figure it out, hopefully the parameter answer will be the ticket

Link to comment
Share on other sites

John,

Obviously there's no pcmcia card slot in the front of the control as you could run the tool from a sub.

But depending on the control/year, there maybe a pcmcia slot in the back (control cabinet). Maybe worth a look.

:cheers:

Were this a customer that I was onsite with, that would have already been done, however, this is a remote customer some 3k miles away

 

So while I can suggest it, and I have, there's not much beyond that and working with them that I can do

Link to comment
Share on other sites

I am at a customer right now that just got bit in the !@#$%$ with this issue with a Fanuc 16i,

 

I tried adjusting minimum arc length values and it did not make a difference.

 

The culprit was the break arcs at 180 setting in the control definition. Since he is using IJ's, full arcs or > 180 are not a problem.

 

 

The latest Cimco Edit does not show the problem, it just ignores that bad line, when I save as DXF it shows a gap.

 

 

N2730 X4.3176 Y15.648 I1.3646 J.0025
N2740 X4.3175 Y15.6466 I-1.3646 J-.0025 bad line
N2750 X3.1841 Y14.3011 I-1.3643 J-.0009

 

 

post-867-0-96298700-1414506184_thumb.jpg

post-867-0-46504600-1414506186_thumb.png

post-867-0-44401800-1414506188_thumb.jpg

bad code.txt

Link to comment
Share on other sites
Guest MTB Technical Services

Glenn, your output is valid meaning that it can run without error.

I have checked it with several different systems.

CIMCO may be having an issue with it.

I was never a fan of their backplotter.

 

However, there IS a rounding issue that is created by the control definitions and the post itself.

Notice the 0.0001 difference in the X values in your highlighted code.

The I values have the same magnitude but the X values are different by 0.0001.

This isn't correct and is the exact cause of the problem at the machine.

Parameter #3410 handles this.

 

If you change the X value to X4.3176, the machine error will disappear.

 

There is clearly a Mastercam issue related to arc length and breaking arcs at 180 degrees.

I would recommend people also use the error checking options for the arc length and radius in the control def.

This rounding error seems to only occur at these points.

 

If you are going to use I&J, setting Parameter #3410 to a greater value will eliminate the issue on the machine.

Depending upon the setting in #3410, #3403 may apply as well.

 

I haven't seen this with any program I've generated since 2008 because I always check the machine parameters

and adjust them accordingly. The value needs to be slightly greater than the minimum resolution of the machine unit system.

Link to comment
Share on other sites
  • 2 weeks later...

Hi guys,

 

I've also had this problem this week at a 2D HST FILTERED toolpath. The filter made "milions of arcs" and one of then made the loop. Fortunately the toolpath was at a high Z and the loop simply stopped on the proximity of the machine...

What I did was changed bit #5 (QCR) of parameter #5008 from ZERO (the FS16 format) to ONE (the FS15 format). The program continued properly. Give it a try. You can find more info in the Fanuc parameter guide. I did this on the 0i-MB. Let us know if it worked and what you think about it....

 

P.S. From the  Fanuc parameter guide:

"FS0 (FS16) and FS15 determine the travel distance in different ways if the

radius of arc at the start point of circular interpolation is different from that

at the end point (if the end point is not on the arc). By this parameter, the

method of determining the travel distance of circular interpolation can be

selected."

Link to comment
Share on other sites
Guest MTB Technical Services

Hi guys,

 

I've also had this problem this week at a 2D HST FILTERED toolpath. The filter made "milions of arcs" and one of then made the loop. Fortunately the toolpath was at a high Z and the loop simply stopped on the proximity of the machine...

What I did was changed bit #5 (QCR) of parameter #5008 from ZERO (the FS16 format) to ONE (the FS15 format). The program continued properly. Give it a try. You can find more info in the Fanuc parameter guide. I did this on the 0i-MB. Let us know if it worked and what you think about it....

 

P.S. From the  Fanuc parameter guide:

"FS0 (FS16) and FS15 determine the travel distance in different ways if the

radius of arc at the start point of circular interpolation is different from that

at the end point (if the end point is not on the arc). By this parameter, the

method of determining the travel distance of circular interpolation can be

selected."

 

Just a note.

This parameter doesn't exist as QCR in the current Oi-M(D) or 30i series documentation.

I suspect it has been obsoleted by FANUC.

Link to comment
Share on other sites

JP whatever happened with this customer? was it the fanuc parameter? thanks Tim!! i will change those parameters in our 18i and 31i controls since this has happened

to me in the past. it always turns out that x,y,i, or j is off by .0001 but plots fine in cimco and runs fine on a fadal (go figure, those fadals)

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...