New Fagor controller does not like smoothing

I have a new router with a Fagor 8037 controller. I had some problems early on with the machine doing some weird moves violating the work. It machined right through the center of a boss. (all 3d work) If I ran through single block it did not violate the job. However anything past 10% feed override it gave a counterclockwise rapid instead of a clockwise cut in this area.

I spoke with Tech support at my supplier and he questioned why my program was outputting G2s and G3s. I told him I used smoothing in my Cam software (HSMWorks) to minimize program size and that my other router ran much more smoothly and avoided jerky movements using smoothing. He told me to set the software to just use G01s. This solved the crashing issue and works reasonably well with geometry that has straight sections in it to allow the controller to catch up. However cutting round parts or larger parts with complex geometry the machine is jerky even at 60% feed and I get a terrible finish. I took a risk and ran smoothing on a semi finishing toolpath tool today and I got a better finish than my finishing toolpath. The finish is all dimpled like a golf ball but way more dimples. I am almost positive I am getting Data starving.

Is this a common issue with this controller? All my jobs are 3D machining and I need to be able to run this machine at a decent feedrate with a good finish. I would prefer to use smoothing as the files are considerably larger and they are taking forever to load on the machine. As well it is something I have to make sure I change in my settings in HSMWorks. I am working up a new set of templates with smoothing turned off.

Is there a parameter that can be changed on the controller to allow it to take the smoothing toolpaths? Or another solution? I will be contacting the router manufacturer next week about the finish as I am sure there are parameter changes that will help but I would love to have a little more information before talking to them.

Post Library for Fusion 36 and Autodesk HSM | Autodesk HSM did you try this post?

WARNING!!! completely useless and sarcastic post to follow..

A Fagor control doing things you don't expect it to??? NOOOOO???!!!????

Start yourself a notebook, and when you figure out what the hell the control
is doing, write it down..

I'd write more but I got to go take a Pee001=K-weeweetime.

Hi Pattnmaker:
Even with the sarcasm, I believe BobW has it right.
You're describing a failure of the control to consistently process the G code it is being given.

If you can completely alter the response to the code just by turning the feedrate up a bit, you have a failure to send the correct signals from the control to the servomotors and the issue appears to lie in how the processor responds to a G2 or G3 input where the response depends on other statements within the code to send the proper current to the motors at the proper time.

The reason you are able to cut more successfully with just G01 in your code is that it is less ambiguous, having only a start point an end point and a linear path to calculate.
It stutters because the control can't cope with the acceleration and deceleration needed at each end of each linear statement so the control accel decel subsystem is not coping with the rapid inputs from short linear moves in quick succession but it still knows where to go and when to stop.

Calculating what to do with an arc statement involves more input information about the direction, the radius, the center point and whether to make a quadrant move or a full circle.
A failure to respond consistently to an unvarying input means the controller is dropping bits of the information it needs as soon as the demands on it go up, and increasing the feedrate is such a demand.

Sad to say, I believe your Fagor controller is hooped; I doubt tuning and doodling it can ever fully eliminate the problem and there is nothing you can do with the code or the post to fix it.
Some claim with some justification apparently, that a Fagor control is a piece of shit that will never work properly.
I've never run such a machine so I can't attest to the truth of that though.

However I do have a Bridgeport DX32 control on a Defiance, and it pulls weird shit like this on me too, so I can't do surfacing on it.
The behaviour is almost exactly as you describe; in Bridgeport's case they lost their ass in a class action lawsuit over the control's deficiencies.
There's probably a new machine or a new control in your future if you really need it to be better than it is now.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

converterking said:

Post Library for Fusion 36 and Autodesk HSM | Autodesk HSM did you try this post?

Click to expand...

I believe that is the post I was provided with and I spent weeks playing wack a mole repairing the problems with this post. The first several problems were with the post being a 5 axis post. The machine would not work freeze up or in one case crash. I would send the code to the manufacturer with a description of the problem and they would tell me the problem which I would then have to get Nexgen to fix on the post.

The machine actually came with a one year subscription to Fusion but I have been working 7 days a week and have not had a chance to try the machine with Fusion. However I have been told the Post is the same so I wonder how well the machine would work using Fusion.

All the troubleshooting with the machine has made the 7 day a week problem worse when it was supposed to make it better.

implmex said:

Hi Pattnmaker:

Sad to say, I believe your Fagor controller is hooped; I doubt tuning and doodling it can ever fully eliminate the problem and there is nothing you can do with the code or the post to fix it.
Some claim with some justification apparently, that a Fagor control is a piece of shit that will never work properly.
I've never run such a machine so I can't attest to the truth of that though.

However I do have a Bridgeport DX32 control on a Defiance, and it pulls weird shit like this on me too, so I can't do surfacing on it.
The behaviour is almost exactly as you describe; in Bridgeport's case they lost their ass in a class action lawsuit over the control's deficiencies.
There's probably a new machine or a new control in your future if you really need it to be better than it is now.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Click to expand...

This is a Brand new machine and I had better be able to do surfacing with it as that is 99% of my work. I do know adjusting some acceleration deceleration and look ahead parameters helped with my first machine. So while I was hoping to be able to use smoothing hopefully I can get smoother results while using only G01s.

The first picture was from a job a week ago the second yesterday at 60%feed override. It is much better but it is still pretty rough. (the cusps at the bottom of the picture were cleaned up in the next toolpath)

Hi again Pattnmaker:
You wrote:
" It machined right through the center of a boss. (all 3d work) If I ran through single block it did not violate the job. However anything past 10% feed override it gave a counterclockwise rapid instead of a clockwise cut in this area. "

"However I have been told the Post is the same so I wonder how well the machine would work using Fusion."

If what you say in your first statement is true, IT'S NOT YOUR POST OR YOUR CAM SYSTEM...YOUR MACHINE IS FUCKED!!
It's seeing exactly the same code when it rapids through the job as when it single blocks without problems.
What it's not doing is responding the same way as soon as you give it it exactly the same instructions but with less time between them.

Playing with different posts is not going to fix this. EVER!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

The older ones anyway, (8020,8025) would never work with
IJK values, only Radius. G2 or G3 with an I J K value would only result in a cryptic error message when the program got to that line.

Not sure about current support from Fagor regarding programming, but 10 years ago any questions about programming seemed to be like talking to a tech that's never programmed any code on any of their controls. Email would come back "See page # in the programming manual"......and page # would be the page that had the G code you were asking about......big help.......NOT.

Good luck to you ....

On the plus side, if the basic machine is actually upto it drive and servo wise its a prime candidate for a control refit, because theres masses of alternative controls out there that are a very long long way away from being the limiting factor in surfacing moves. The limits should very much be down to the simple torque the axis servo's can deliver to move things fast enough. That in turn is literally down to how much you want to spend on servo's and drives.

Computationally most pentium class processors of the last decade should be able to handle the calculations for differing lines of G02 or G03 moves in the range of hundreds of thousands of lines of G code a second. Certainly the limitation is how fast you can make a movement system keep up, it should not be how fast a controller can calculate the moves any more.

Can't believe a machine supplier is recommending G01's only as the fix,

Seems like the old controls were 8086 processors.
Wonder if they're still using them!

Pattnmaker said:

.... However anything past 10% feed override it gave a counterclockwise rapid instead of a clockwise cut in this area.

Click to expand...

It would be an interesting bit to find out what this machine has for drives.

Stepper motors are notorious for losing counts or just stalling out at higher speeds.

If the machine has steppers (common on budget routers), I'd figure out how to get rid of it and buy something with servos.

We recently got a lathe with a 8037TS and it definitely has its quirks. My suspicion is that your troubles are from G05/G07 (round corner/square corner). G07 will force the machine to stop momentarily at every point you program whereas round corner will round all those corners off. As an example, I had G05 active when I was finished turning a profile and the next thing was to rapid and clear the park in Z to +1” then go to position for the next tool (this is a gangtool lathe so no turret). Initially, it headed toward z+1” but ROUNDED the corner to get to the next tool and went right into the part.

There is however, a G50 which is called controlled corner rounding which you can set vector limits to how much maximum rounder rounding you want.

I suspect if you search your programs you will find G07 where the machine is stuttering while machining and G05 where you are taking out that boss.

These are modal commands, and I find they can be very helpful if you know when and where to use them.

This is of course, if the 8037 M control had the same codes at the 8037 TS.

Vancbiker said:

It would be an interesting bit to find out what this machine has for drives.

Stepper motors are notorious for losing counts or just stalling out at higher speeds.

If the machine has steppers (common on budget routers), I'd figure out how to get rid of it and buy something with servos.

Click to expand...

This is not a "budget" router. Not high end but not a budget machine either. Servos and ball screws on all axis. I thought I was better off getting an industrial controller on my new machine. So far I am getting better finishes on my Windows based router (also servos and ball screws)

The new machine seems to be capable of much higher feeds than my old one especially in the z axis. On jobs that the controller can keep up it is much faster and is a solid machine. On the more simple geometry (but not round) jobs I am getting a good finish.

I remote accessed the shop computer and checked the programs for G5s and G7s not G7s and the only G5 was at the beginning of the Adaptive toolpaths. The problem was during the contour toolpath. Thanks anyways it was worth a look.


I will have to check into IJK values. Not really sure what they are and I will have to zero into the program locations.

The radius or ijk, inc or absolute is set in your post.

Pattnmaker said:

This is not a "budget" router. Not high end but not a budget machine either. Servos and ball screws on all axis. I thought I was better off getting an industrial controller on my new machine. So far I am getting better finishes on my Windows based router (also servos and ball screws)

The new machine seems to be capable of much higher feeds than my old one especially in the z axis. On jobs that the controller can keep up it is much faster and is a solid machine. On the more simple geometry (but not round) jobs I am getting a good finish.

I remote accessed the shop computer and checked the programs for G5s and G7s not G7s and the only G5 was at the beginning of the Adaptive toolpaths. The problem was during the contour toolpath. Thanks anyways it was worth a look.


I will have to check into IJK values. Not really sure what they are and I will have to zero into the program locations.

Click to expand...

G05 is modal so it is active through all of your program after that point and even continues to be active in the next program until you shut the machine off. I think you need to investigate these codes more. Run some rapid moves above your part that have x and y coordinates to see better how it effects the actual path. You solution will be with a G50 code. G05 will not be accurate but run fast. G07 will stutter like crazy.

I will try re cutting the corebox that we had the boss machined through with smoothing turned on but I will change the G5 to a G50. I will cut a piece of wood that is just higher than the boss that is cut through. Do I need anything added after the G50? Does G50 turn off G5?

Pattnmaker said:

I will try re cutting the corebox that we had the boss machined through with smoothing turned on but I will change the G5 to a G50. I will cut a piece of wood that is just higher than the boss that is cut through. Do I need anything added after the G50? Does G50 turn off G5?

Click to expand...

G05, G07, G50, and G51 will all cancel each other. G50 does not require any other values like G05 and G07. It sets corner rounding limits through your parameters.

If G50 helps then you may want to research G51. I haven’t done any programming with it because I only have a simple 2 axis lathe so I cannot help much. But it is like G50 with look-ahead and accel/decel limits I think.

Hi Pattnmaker:
Can you duplicate the incorrect behaviour at will?
You said it would receive a G02 or G03 command and execute it correctly so long as the feedrate override was set to less than 10% or if you ran the program in single block mode.
Are you describing a total feedrate of 10% of what was programmed or 110% of what was programmed?

When it crapped out and ran the code wrongly, you said it reversed direction and made a full arc through the workpiece but at a very high feedrate.
Think of what it would have to do to execute a move like that.
It still needs to co-ordinate the two axis motors to make an arc and the co-ordination is quite sophisticated.
It needs to put a lot more current into the motors to make the feedrate go up.
This is not the behaviour of a voltage spike or a failing component; it's also not the behaviour I'd expect from a corner rounding code inappropriately set...it's a whole new behaviour in which the control has interpreted the code it got completely wrongly; but it did interpret it or else it would have given a following error alarm or just done an uncontrolled runaway.
The fact that it does it under certain conditions and does not do it under others while using exactly the same code makes it hard to believe it could possibly be the code that's at fault.

If you program a very simple 2D contour can you make it behave this way?

If you program several arcs in succession, does it execute them all correctly or does it go strange on you?

If you program a rectangle with rounded corners and lead-in lead-out arcs does it go strange then?

I'd try out those very simple examples and then try to duplicate the behaviour by manipulating the feed override.
Write the code by hand and then go to town with it.
Write it also with the CAM system you're using and see if that makes a difference.


Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Using smooothing 99% of the job cuts just fine. Then one job I got this weird cut through the boss cut. The corebox was 2 impressions exactly the same. I did a semi finishing toolpath with .010" stock left and a .1 stepover. The boss was cut through on one of the 2 impressions on the semi finishing toolpath but not the other. Then on the finishing contour toolpath both bosses were cut through. The problem is I don't know when the problem will manifest. This specific time the toolpath was supposed to go into an acute corner and then rotate out of the corner. Imagine a round boss close to an edge and there was not enough room for the end mill to go between the wall and the boss. I had it cut into a wall during an adaptive toolpath as well. This triggered a spindle overload so there was not much damage. The weird thing is the load on the spindle would not have been that high. I regularly take much bigger cuts with that endmill. One of the techs at the manufacturer suggested a post change that just made the problems worse.

I tried adding a G 50 to the program for this corebox and ran it. The post I am using puts in a G51 so the G50 turned the G51 off. It did not cut through the boss, however with no look ahead turned on it almost came to stop in all the corners it was very jerky in a section with Radial draft and when it go the the bossed it was jerky and painfully slow. Thanks for the suppestions anyways.

I am going to have to spend a bunch of time reading the manual to see if there is anything of use in there but I don't want to make any parameter changes without speaking to the manufacturer especially as this may void my warranty. Until I have time to really dig into it I guess I will have to just keep smoothing turned off and the feed slow on geometry that does not have straight sections that allow the controller to catch up.

This corebox was long ago delivered and the odds of me ever having to make another exactly the same is very slim but as I know where the problem manifests it is a good test subject.

Pattnmaker said:

Using smooothing 99% of the job cuts just fine. Then one job I got this weird cut through the boss cut. The corebox was 2 impressions exactly the same. I did a semi finishing toolpath with .010" stock left and a .1 stepover. The boss was cut through on one of the 2 impressions on the semi finishing toolpath but not the other. Then on the finishing contour toolpath both bosses were cut through. The problem is I don't know when the problem will manifest. This specific time the toolpath was supposed to go into an acute corner and then rotate out of the corner. Imagine a round boss close to an edge and there was not enough room for the end mill to go between the wall and the boss. I had it cut into a wall during an adaptive toolpath as well. This triggered a spindle overload so there was not much damage. The weird thing is the load on the spindle would not have been that high. I regularly take much bigger cuts with that endmill. One of the techs at the manufacturer suggested a post change that just made the problems worse.

I tried adding a G 50 to the program for this corebox and ran it. The post I am using puts in a G51 so the G50 turned the G51 off. It did not cut through the boss, however with no look ahead turned on it almost came to stop in all the corners it was very jerky in a section with Radial draft and when it go the the bossed it was jerky and painfully slow. Thanks for the suppestions anyways.

I am going to have to spend a bunch of time reading the manual to see if there is anything of use in there but I don't want to make any parameter changes without speaking to the manufacturer especially as this may void my warranty. Until I have time to really dig into it I guess I will have to just keep smoothing turned off and the feed slow on geometry that does not have straight sections that allow the controller to catch up.

This corebox was long ago delivered and the odds of me ever having to make another exactly the same is very slim but as I know where the problem manifests it is a good test subject.

Click to expand...

It was definitely a spindle overload? Could it be that the actually toolpath deviated too far from programmed toolpath?