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:

Fanuc controls, short arcs cutting as full arcs.


Recommended Posts

Here we go again and still stumped by this. Please let me explain as well as I can. Another customer has called complaining that a small arc in a really dense program is actually deviating and cutting a full circle. I had another customer call about the same thing about a year ago. This latest event happened on a Fanuc 21i and the previous case was on a Fanuc Oi control. I had this happen to me way back in the 90's and scrapped 2 $30,000 mold cores. One was an 11M Fanuc and the other was a brand new 16i Fanuc.

In all cases arc fitting was used. In all cases verify was used and back plotting was used. In the most recent 2 cases I was not able to duplicate it on our showroom machines with the customers program. It did not matter whether I's and J's were used or whether R's were used to define arc center. It's not the CAM program because in all cases a different CAM program was used. Mastercam in the last two cases and Unigraphics in the others. Like I said, verify and back plotting did not show anything. In the year ago instance the customer marked the offending arc in his program. It had a radius of 92" and an arc length of only .0002". I still could not duplicate this on our machines with the same control.

The latest customer stated that this same program ran fine on a machine that used G05.1 but the offending control did not have any look ahead. The only way I fixed it was NOT to use arcs but that is only a work around and we still have no cause.

This has stumped me for years and is bugging the crap out of me. Fanuc claims no knowledge of this. Has anyone seen this scenario, ever? I would like to pin this down one way or another despite what the news may be, god or bad.

Thanks,
Paul

Link to comment
Share on other sites

I did post this on Practical Machinist. I get the same responses all the time. Break your arcs into quadrants and stuff like that. These are arcs that may only have a portion of a degree of rotation. Yet the control wants to complete e full circle. Totally defies the physics of the machine and control.

 

Paul

Link to comment
Share on other sites

Break arcs into quadrants would not fix a 92" arc with a length of .0002".

 

Not really helpful I guess, but VERICUT software got many enhancements in regards the detection of Fanuc bad arcs in the past 2 years, specially to deal with these cases where the customer was getting a gouge but the CAM system was not detecting it. Basically CGTech received the offending code and figured out how to reproduce them. It may be the answer you´re looking for.

Macro: FanucArcLengthWarning
Function —Miscellaneous
Status — ACTIVE
Comment — Added V7.2.3
Inputs —
Text: Not Used
Value: 0 = disable / 1 = enable (Default)
This macro enables comparing two different Fanuc arc length solutions (one implemented in the older FS15 and the other in the newer FS16 CNC systems). When enabled, the resulting arc motion produced by the commanded arc’s start and end locations are compared between the two different Fanuc methods. If the two methods determine different solutions (one chooses long arc, the other chooses short arc) then the following warning message is sent to the logger:
"Warning: Arc start and end points may produce undesirable motion on Fanuc controls, at line …"
This does not apply to circle motions where the start and end points are coincident and produce a full 360 degree motion.
Link to comment
Share on other sites

^^^^good to hear Vericut is still working on it^^^

 

i had it happen in 2004ish. I had MC output I/J arcs set to break into quadrants.. joggle in thin walled part (for airbus A380) was less than cutter radius.

 Tool blew through wall, so it either tried to do a full circle or complete the big circle instead of the small one.

Verify, backplot AND vericut could no reproduce it.

 

changing to R's fixed that program......

 

this was a mori SH500, not a doosan.

Link to comment
Share on other sites

Actually I've seen this before.  It was a rounding error caused by a bad control definition and it made the machine do the opposite.  Instead of a full circle, I got an extremely small arc segment.  Basically, the end point of the arc was just past the start point of the arc after the code was posted due to rounding error.  However, in the MCX file, the start and end points were identical.  This caused basically no movement at all.  If I were you, I would look at all resolution settings, the machine tool parameters as well as the control definition.

Link to comment
Share on other sites

I had a real gouge with our FANUC and Vericut a couple years back...they made several software updates from our problem. They even sent a guy out and video tapped the machine and control!

 

The minimum arc radius in Mastercam control definition was too small and the control just did a complete arc unexpectedly.

 

Now inn Vericut it still verifies okay but you get a warning...if you turn that option on of course...WTF do you need to turn that option on?

Link to comment
Share on other sites

Here we go again and still stumped by this. Please let me explain as well as I can. Another customer has called complaining that a small arc in a really dense program is actually deviating and cutting a full circle. I had another customer call about the same thing about a year ago. This latest event happened on a Fanuc 21i and the previous case was on a Fanuc Oi control. I had this happen to me way back in the 90's and scrapped 2 $30,000 mold cores. One was an 11M Fanuc and the other was a brand new 16i Fanuc.

 

In all cases arc fitting was used. In all cases verify was used and back plotting was used. In the most recent 2 cases I was not able to duplicate it on our showroom machines with the customers program. It did not matter whether I's and J's were used or whether R's were used to define arc center. It's not the CAM program because in all cases a different CAM program was used. Mastercam in the last two cases and Unigraphics in the others. Like I said, verify and back plotting did not show anything. In the year ago instance the customer marked the offending arc in his program. It had a radius of 92" and an arc length of only .0002". I still could not duplicate this on our machines with the same control.

 

The latest customer stated that this same program ran fine on a machine that used G05.1 but the offending control did not have any look ahead. The only way I fixed it was NOT to use arcs but that is only a work around and we still have no cause.

 

This has stumped me for years and is bugging the crap out of me. Fanuc claims no knowledge of this. Has anyone seen this scenario, ever? I would like to pin this down one way or another despite what the news may be, god or bad.

 

Thanks,

Paul

 

Hi Paul,

 

I'm not sure if I can help specifically in regards to your issue, but I might be able to shed at least a little light on the issue.

 

Dealing with small arcs like this is always a cause for concern. The issues stem (as you've so painfully discovered) from the control incorrectly swinging the "wrong way", or the machine tries to complete a full circle.

 

The first thing I know is that there is no such thing at two "identical" machines. This is due to the fact that each machine has a control unit that is setup using "Parameters". The individual bits for each parameter number (and the options purchased on the machine) would have to match exactly, and not only that, but the build dates in the factory, and the configuration of the electrical components (things like specific capacitors and resistors) would need to also match.

 

This is often due to different Applications Engineers having a preference on how the machine is setup, or in some cases just different options being purchased for the build. As an example, we've got 3 different Mazak Integrex e-1850 machines on our shop floor, and each one has subtle differences in how the control is configured. We have done some work to standardize the codes we use on all three machines, but we still occasionally run into issues with Parameters being set differently between the machines. It can be a real nightmare to figure out, as you are seeing.

 

Check Parameter #3410 - Tolerance of Arc Radius

 

This parameter can have different values, depending on if you are in Inch or Metric increment, and what the resolution of the control is set to. (.001, .0001, or .00001 inches).

When a circular interpolation command (G02, G03) is executed, the
tolerance for the radius between the start point and the end point is set. If
the difference of radii between the start point and the end point exceeds the
tolerance set here, a P/S alarm No.20 is informed.

NOTE
When the set value is 0, the difference of radii is not checked.
In the HPCC mode, a check is made for a difference in the arc
radius even if the set value is “0” (with allowable limit = 0).

What about High Speed Modes? Depending on if HSM was used, could there be a difference in the maximum "corner rounding radius" allowed?

 

You can set some parameter settings inside Mastercam's Control Definition to limit the size of the arcs you are allowed to create. The defaults actually allow you to create some pretty small arcs. An Arc length of only .0002 is especially tiny on a 92" diameter. The control is probably interpreting those points as so close together, as to actually be a full circle. So your machine is dutifully trying to swing that arc, even though you just wanted the small portion.

 

I would recommend setting the options in Mastercam to make the minimum Arc Length something like .004 (or bigger), and set the minimum radius to the same. (.0005 is the default I believe, and is too small for my liking.) This setting, more than any other, is allowing Mastercam to create these arcs with small distances between the endpoints.

 

When I have investigated this issue for CNC Software in the past (I worked in the Post Department for about 3 years), we typically found that if you plotted out the tool path locations down to 10 millionths (.00001), that the arc endpoints would often be off, but not enough for the settings to break the arc into lines. Sometimes you would have a center point, or an endpoint of the arc be off by .000044. Not enough to cause Verify or Backplot any issues, but certainly enough to ruin your day when the machine decides to go the wrong way on you.

 

What type of path was generating the small arc? Is this a surface roughing/finishing routine, or are you just Contouring something? Is Cutter Comp being used? Are the Cutter Comp settings exactly the same? Is there a default "Corner rounding radius" or "Corner rounding mode" that is active on the customer's machine?

 

Sometimes how you play with the filter can make a big difference on how "Filtered" the path is. One of the biggest mistakes I see people making is not using enough Tolerance for their operations. They crank the filter down to .0001 on everything, without realizing that not only does it increase the time to generate the path, but they also get these tiny arcs that cause problems. I will often use .006 to .05 for my "Total Tolerance", depending on how much stock I am leaving. Usually I shoot for about 10% of my Stock to Leave value. Then I will make the "Cut Tolerance" more accurate, and make the "Filter Tolerance" a little "looser", to be able to fit bigger arcs to the path.

 

Also, the other place we saw problems was when a path would generate a G02 arc, then a small G03 arc, followed by another G02 arc. (or switch G2/G3 in that last statement). The point being that the path was switching back and forth between CW/CCW arcs in rapid succession, and the arcs in general are have a fairly short "Arc length". So bumping up that minimum Arc Length tolerance is critical.

 

In the "Arc settings" page of the Control Definition, make sure "break at 180" is turned on, unless you want break at quadrants. For the 21i, you should be able to support "helix in XY plane only". On the "Arc error checks", there are 5 check boxes on the lower right side of the page. Make sure you have them set to "On", "Off", "On", "Off", "On". So the first, third, and fifth boxes should be set to "On", and 2 and 4 are turned off. Paul explained to me why this was important once, but I never did remember the exact details. Something about the way that MP was setup internally and how the settings are used during actual tool path generation. Anyway, if you don't have the correct Arc Error check settings, you're gonna have a bad time.

 

So, as to "why does this keep happening", I would suggest trying to figure out the parameter settings that are different between your machine on the shop floor, and the machine with the issue. Is it possible to get someone from Fanuc out at the customer's site, and to run the program without a part loaded to try and trace down the behavior?

 

Sorry for throwing out a bunch of "have you thought about this" type questions, but I've been dealing with the same issues on and off my whole career. Still do. So anything you find out regarding the issue would be much appreciated as well. It does seem to creep up more often on the older Fanuc controls. I don't see it as much on the 30 series as I do the O, 6, 16, and 21 series of control.

  • Like 2
Link to comment
Share on other sites

WTF do you need to turn that option on?

 

Go to 'Configuration -> G-Code Processing -> Expand 'Events' -> Expand 'Start of Processing' -> Expand 'Global' -> Add the macro 'FanucArcLengthWarning' with the field 'Override Value' set as 1

 

This will make sure it is enabled when you push play.

Link to comment
Share on other sites

Go to 'Configuration -> G-Code Processing -> Expand 'Events' -> Expand 'Start of Processing' -> Expand 'Global' -> Add the macro 'FanucArcLengthWarning' with the field 'Override Value' set as 1

 

This will make sure it is enabled when you push play.

 

Problem is they apply that to their other controls that don't have this problem. You have to fight with them to remove it from a Siemens and Okuma controls. Lost one week going back and forth with a 840D and another week with a P300M. Both kept reporting back this Fanuc error from HST toolpaths. Had to go out to the machine and run the problem area before the customer would say maybe the code is good and Vericut is giving a false alarm. Glad they have the check, but not every control has the same issue.

Link to comment
Share on other sites

Problem is they apply that to their other controls that don't have this problem. You have to fight with them to remove it from a Siemens and Okuma controls. Lost one week going back and forth with a 840D and another week with a P300M. Both kept reporting back this Fanuc error from HST toolpaths. Had to go out to the machine and run the problem area before the customer would say maybe the code is good and Vericut is giving a false alarm. Glad they have the check, but not every control has the same issue.

 

Not sure about that. You can have this on a per machine basis. It´s not a global setting.

Link to comment
Share on other sites

Glad you brought this to the surface Ron:

 

In order to have VERICUT calculating tolerances for start/end points the same way your control does, go to 'Configuration -> Control settings -> 'General' tab and set the value of the field 'Calculation tolerance' with the value that your control is using.

 

In a Heidenhain control, this value is typically 0.016mm, tops, and is set at the parameter MP7431. But the machine builder can set that a bit tighter, as well. A well configured VMC (Vericut Machine Configuration) with a Heidenhain control uses in this field the same value used in MP7431.

 

In a Fanuc control, that value would come from parameter 3410.

 

Now the surprise:

 

Normally, the macro 'FanucArcLengthWarning' is not included in the default controls from VERICUT´s library, so unless you have it explicitly added to a control, odds are high that you are not using it.

 

VERICUT controls are typically supplied by CGTech with a value of 0.001" (0.025mm) in this field, since CGTech is unable to know what value your control is using in real life. 99.9% of users never change this value in a VERICUT control, so with a larger tolerance the software may not reproduce exactly how your machine behaves and overlook real problems or issue false alarms.

 

As the real world is metric, ( :harhar: ) I use a value of 0.01mm in my controls when I don´t know what tolerance the control is using. But in fact, I always manage to find this value in all controls we have here and have VERICUT using the same value. The tighter you set this in the control and VERICUT, the less tolerant to bad arcs both will be.

 

Not a definitive answer about it but perhaps can be of help.

 

JM2C

Link to comment
Share on other sites

Thanks everyone. All good stuff here. A little more background. All 4 instances that I have been directly involved in, the toolpaths were high speed tool paths over 100 IPM. 2 from Mastercaam and 2 from Unigraphics back in the 90's. The two older events were on a Mori with 11M and a new Makino with 16i. Scrapped 2 very expensive mold cores. Of course the programmer (me) got blamed. Fast forward about 20 years, I have a high stake in solving this. These last two events, one was a Doosan with an Oi control and the other is an older Doosan with a 21i control. Other than the 16i, these aren't controls you would normally associate with good high speed machining performance. The latest customer states he can run this program safely on a machine with G05.1 turned on. The offending machine, 21i,  has no advanced look ahead options. Last year I reposted a customers offending operation in my MX setup, sent it to him and it ran fine for him. But I still don't think it is entirely a Mastercam issue.

 

I agree with the above about setting the tolerances too low and allowing such small arcs.

 

Attached are two files. The offending G-Code file and a pic of the resulting part.

 

Thanks All, I appreciate the help,

 

Paul

 

 

2D HIGHSPEED FOR DOOSAN (2).zip

2D-High Speed.zip

  • Like 1
Link to comment
Share on other sites

Glad you brought this to the surface Ron:

 

In order to have VERICUT calculating tolerances for start/end points the same way your control does, go to 'Configuration -> Control settings -> 'General' tab and set the value of the field 'Calculation tolerance' with the value that your control is using.

 

In a Heidenhain control, this value is typically 0.016mm, tops, and is set at the parameter MP7431. But the machine builder can set that a bit tighter, as well. A well configured VMC (Vericut Machine Configuration) with a Heidenhain control uses in this field the same value used in MP7431.

 

In a Fanuc control, that value would come from parameter 3410.

 

Now the surprise:

 

Normally, the macro 'FanucArcLengthWarning' is not included in the default controls from VERICUT´s library, so unless you have it explicitly added to a control, odds are high that you are not using it.

 

VERICUT controls are typically supplied by CGTech with a value of 0.001" (0.025mm) in this field, since CGTech is unable to know what value your control is using in real life. 99.9% of users never change this value in a VERICUT control, so with a larger tolerance the software may not reproduce exactly how your machine behaves and overlook real problems or issue false alarms.

 

As the real world is metric, ( :harhar: ) I use a value of 0.01mm in my controls when I don´t know what tolerance the control is using. But in fact, I always manage to find this value in all controls we have here and have VERICUT using the same value. The tighter you set this in the control and VERICUT, the less tolerant to bad arcs both will be.

 

Not a definitive answer about it but perhaps can be of help.

 

JM2C

 

The Control and Machines for Vericut were built and made by CG Tech in both instances for a customer who was under maintenance. The status quo from a different CAM System was to just linearize everything when they were seeing that error. We went back and forth for a week trying to sort out how the same settings had run other machines in Mastercam with no problems would not work on that machine. It was not until we would not accept it was a Mastercam error and it had to be a Vericut issue was it finally given the attention we thought it deserved from the very beginning. It was addressed and once it was the error has not come back since. CG Tech makes a good product I am not saying it doesn't, but in this instance it had been around for years and was not addressed till an outsider said nope it has to be something other than the CAM Program. That cost the customer and our company a week of lost time going back and forth trying to sort all of that out.

Link to comment
Share on other sites

The Control and Machines for Vericut were built and made by CG Tech in both instances for a customer who was under maintenance.

 

Even CGTech guys seldom asks for or change that value. I´ve purchased almost a dozen of machines from them in the past 7 years and they never bothered to mess with the 'Calculation tolerance' in the control of a single VMC.

 

I find bugs in VERICUT every other week, and some of them take a very long time to be addressed. Most don´t hopefully. I do fierce follow up on my issues, and they respond accordingly.

 

Unfortunately CGTech business model would make useless for them to have machine tools in their basement like CNC SW. By the way CNC was a pioneer in having their own R&D shop - Before them, only Delcam, which has by the way a shop that is also a business unit doing external work.

 

So the only way CGTech has to fix issues is hearing from the customers and with all facts and data in the table. Once you can give them evidence, they are keen to address the issues.

Link to comment
Share on other sites
  • 5 months later...

Has anybody successfully been able to solve this issue at post level ?

We had this issue occur on a recent big $$$ part.

Vericut had given a warning 'small arc length - undesirable results may occur', but our junior programmer didn't see any harm in continuing, even with this error.

In our case, it has nothing to do with the controller (FANUC 31i). It's MasterCam's post pro that generates a huge I & J  (nearly 360 degrees) at a location where there is a tiny arc. Programming the same cut-out (with the tiny arc) in SmartCam shows no problems after posting. We tried multiple scenarios (cutter comp on/off, arc breakage, different chain generation approaches, etc.

I feel something is fishy in the post and someone must have had this before.

 

Any help or advise in the right direction would be tremendous help - our local CGtech focal can't figure it  out....

Thx

Stan

 

Link to comment
Share on other sites

Hi Stan,

 

I am not an expert, just going from my own gouge experience with our Fanuc Oi-Mb control. I got bitten a few times, even verified with Vericut to be  good code. Vericut sent a guy in to video tape the machine and watch the code. They made several updates to their software to try and capture the problem.

 

The problem they found was the min arc radius was causing the problem. I bumped it up to 0.005"

 

Not sure if this is the cause of your problem or not but just a suggestion.

 

When you do find the cause of the problem it would be great to hear what was causing it.

 

Good luck!

 

John

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

It isn't just 'Min Arc Radius', although that does play a factor. Check the 'Min Arc Length' setting. You should raise that value up bigger than .010 (.25mm). I like to use .020(.5mm), this also helps prevent these small arcs from occurring.

One thing that people forget, or are unaware of, is that each toolpath itself has a Filter, and you can use different tolerances for each path.

So, in my roughing paths, I set the Minimum Arc Radius to .05 - .150, and the Maximum Arc Radius to 100.-250. This can help eliminate those problem arcs, while still letting you swing a .002 radius arc on a finish path.

Some people like to be able to interpolate holes with an endmill that is almost on size. I'm not a fan of that practice, but still think Mastercam should be used to meet your needs.

Link to comment
Share on other sites
  • 1 month later...

Hello,

I know this is old and, no, we have not nailed this down yet to a specific cause. I think Colin might have come the closest though with his remark about minimum arc length. This makes the most sense since the examples I have seen were arc length less than the standard Mastercam tolerance. But this isn't a Mastercam issue although Mastercam can help prevent this from happening. I think the real issue is how a Fanuc control interprets an arc and it's not simply tied to the minimum radius parameter on a Fanuc control. The most glaring example was when the toolpath had a huge radius, say 80 inches. I forget exactly. But the distance from the beginning of the arc to end was about .0002. I think this caused the control to interpret the arc as a complete circle.

I only had this happen to me personally 2 times. Both times ruined very expensive mold cores. Now. as an applications engineer, I have seen it 4 more times. Certainly not often enough to grasp the cause easily. This is over a period of 20 years. Thanks for everyone's input on this. I admit this subject had died down until Colin posted.

Colin, thanks for bringing this up again. I most appreciate you chiming in on an old post like this. Some of these things never die, especially once you get bitten once again.

 

Paul

Doosan Machine Tools

  • Like 2
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...