Fanuc - Advice/Help

[Travis_Buchanan]

I have a Super Shoda Router with a Fanuc 16i-m control. As of lately I am not getting good circle cuts more like eggs. I have always felt that I need to get a Fanuc tec in here and let him tune the parameters on the machine. Cut quality in 3-axis sucks, always has. The shoda rep told me the machine was designed to cut plywood not 3-ax stuff. I have messed with the accel/decell rates and the max arc feedrates in the parameters and it is a little smoother but not much. Does anyone here know if the 16i-m is a good control for 3-ax? I know some controls handle 3-ax better than others. Also what do you think about a Fanuc tec's ability to tune a control to a machine? I have not had good luck with the guys we bought the Shoda from.

[crazy^millman]

Oh yeah but make sure you are using the G5.1 Q1 if it has it. There are other feed foward type functions but James is the Fanuc guy in my book. I have learned alot talking and getting help from him.

 

A test I picked up from a service tech was to program a loop where you travel say a 2 or 3 inch cube at 100 ipm. watch the axis outputs and make sure they stay in sync if they do not then you have some issues with all axis being sync to each other.

 

HTH

[mcpgmr]

Never had a problem with 16im control regarding egg shaped circles. One sugestion would be to check the Lead Comps for each axis if you can. If the Ball screws are worn and the machine is not comped for the wear you might see this happening to your circles.

[Travis_Buchanan]

I am programming G64 with G08 P1. If I set G08 P0 then my tolerances are off. I have never used G5.1 Q1. I have never really understood what the G08 P0/P1 did.

 

G61 = Exact Stop mode

G62 = Auto Corner overide

G63 = Tapping Mode

G64 = Cutting Mode

 

I thought g64 was to run like g62 unless the angle of the next g01 was less than some parameter then do a one line exact position. Kind of like an auto g09, where you need a sharp corner. So how does the g08 affect g64?

[Tim Aydt Prototek Engineering]

Trav, Is your post outputting R's or IJ's?

[Travis_Buchanan]

I use R. No preferance for me the only reason I use R vs IJ is memory space.

[Tim Johnson]

We had to have our last two Enshu's with fanuc 18I controls dialed in. Turned out that they were mistuned when they were assembled. When we ran G05 or G08 they ran good. We sent Enshu our defective parts and they sent a guy in to reset some parameters and now we no longer need look ahead. If your local Shoda rep can't fix the problem you may want to go over their head and call Shoda yourself.

[George_Gerhard]

Travis

the G08P1 is advance preview control.

There is a parameter called feedrate clamp by radius, you may have to reduce this so that the machine will slow down to cut a more accurate circle.

Also parameters 1852 and 1853 are RV1 and RV2 these have a direct effect of the quality of your cuts. Do you also have chatter marks?

Next cut a circle measure it at 12 and 6 oclock

3 and 9, then on 45 degrees such as 2 and 8 and 10 and 4. Which way is the circle out?

I have repaired these problems on many Shodas over the last 18 years

[Jack Mitchell]

George & Travis,

 

Is it possible that this machine is using stepper motors instead of servo motors?

 

The basic thought of closed loop and open loop or direct feedback comes to mind. I also had an issue with AH-HA controllers at one time and had to tweak the control in order to get a round interpolation (whether programmed in quadrants or full circle had no bearing on this).

 

Regards, Jack

[Travis_Buchanan]

George, the machine jerks and bounces real bad during 3 axis cuts, "short straight line segments". I am almost sure the machine needs a good tune up. I was told it wouldn't get any better because it was such a heavy gantry. 8 heads. But I know this to be false as I have delt with routers with as much or more weight being moved around. This is a good machine, 4 years old and run hard, it just needs a good tune up. I just don't know who to get to work on it.

[George_Gerhard]

Travis

Absolutely you need the drives set. This is one of the biggest problems with Shoda, though it is a very good machine, they build the machine and ship it no test cutting.

I dont know how familiar you are with the control but program a 45 degree angle at a feedrate in the metric system (because the machines detect unit is metric)

then check diagnostic 3000 which is following error. X and Y should have the same values.

You can calculate the error using the following formula

fe=fr/60 * 1/gain * 1/detect unit

that is for a straight line, for an angle divide the result by the square root of 2

 

fe = following error

fr = feedrate

the gain is either 3000 or 4000

the detect unit is probably .001 mm

 

rgds

George

 

ps

Mike Olski at GPM should be able to help you

[Jimmy Wakeford from Barefoot CNC]

Travis

Have you thought about using the high feed option in mastercam? YOu could setup the params and let mc do all the speed up slow down stuff.

 

YOu would also have to start drip feeding though cause the programs would be huge.

[Tim Aydt Prototek Engineering]

Trav

I know that from previous experience having your arc output in IJK format will increase accuracy quite a bit

[Travis_Buchanan]

George, Thanks for the help and advice. I am trying to get a hold of a couple of different people right now to come take a look at the machine.

 

Jimmy, I want to get this machine right, it never has been from the start. If I get it tuned up and still have problems then I will try the high feed option.

 

Tim, I can see how that IJK output will let a control do more accurate caculations, but I am cutting wood so we are generally happy with +/- 0.005". All my programs are 4 decimal places so any rounding errors will surely fall within the 5 thou range.

 

So I assume that the 16i-m is a good control for 3-ax work?

[Guest CNC Apps Guy 1]

The 16i-M is an OUTSTANDING control. That is not the issue.

 

Jack, Fanuc does not even make a Stepper Motor to the best of my knowledge.

 

Are you by chance DNC'ing???

 

Travis yes your machine needs to be tuned. Shoda makes a great router but as was stated earlier they don't really tune it for 3 Axis stuff. Not really their fault, they have it set for the largest segment of their market - panel type work, not a lot of detail. My gut instinct is that the behaviour you're seeing is what's called "Data Starvation" or "Servo Lag". It means that the moves are so small, that the control cannot process the moves fast enough so it's hesitating a bit. See, a stock 16i (meaning no SHPCC/AICC, NANO AICC, HPCC, or NURBS) has only 1 block look ahead. Using the Look Ahead Option you get you get 8 (I think), with SHPCC/AICC, you get like 16, with HPCC and NURBS you get 180 block look ahead. Now what all that gobbledygook means is that the control is able to look ahead and judge accel/decel based on what is going on in those blocks. You are better off using I,J,K for precision. If program storage is an issue, look for my Topic about using SRAM/Memory cards as a dataserver. This will save you a TON of $$$$.

 

HTH

[Travis_Buchanan]

Thanks James. I am not dnc drip feeding this control. I do know that I have the G08 P0/P1 option which I think is the 8 line look ahead. Is the G5.1 Q1 option the better look ahead? I am not sure if I have this or not but I will stick it in a prog and see if I get an alarm or not. I may need to upgrade the controler to the hpcc/nurbs option. I am determined to get this machine what it needs to be. I wish you could hang out with us more.

[Tom Dorgan from American Precision]

Travis, Do you have a manual for your 16i control? I may could help you out in this area if you don't.

[Travis_Buchanan]

Yes I have a manual, but I wouldn't know where to start when it comes to tuning the machine.

[George_Gerhard]

Travis

Your company could hire my services and I WILL repair your problem. Please I dont want to sound like I am bragging but I have about 20 years experience with fanuc controls even before the 3 series I was interfacing the 7m, and I know woodworking machine problems very well. I wish I had a quarter for every time I repaired a chattering problem.

[Travis_Buchanan]

George, That may be an option. I am trying to contact a couple of guys I know, but they work for companies that sell/service other brands of cnc routers. I don't know if I can get them in here or not. These guys are local and I have delt with them in the past so I am going to give them a shot 1st but I will keep your offer in mind. It is hard to get a hold of anyone right now with all the holiday maddness going on.

[Guest CNC Apps Guy 1]

quote:

---

...Is the G5.1 Q1 option the better look ahead?...

---

OMG YES!!!

 

You have WAAAAAAAAAAAAAAAAAAAAY more control over acc/dec. I wish I could type as fast as I can think... G5.1Q1 is like an F1 Race car, and G8P1 is like the car in your garage. No $#!+ !!!!! This is what the Hard Milling Mold people use to get superfine finishes on molds that require very little handwork after machining. First things first though, you need to get the servos tuned. Tune them for the max weight you think you will run in the machine. You can always slow things down if you want to machine heavier stuff later on. Once you do that, you can then deternime weather or not you need HPCC or you can get away with SHPCC/AICC which is considerably less expensive. HPCC requires new hardware. You get a 64bit RISC with it. NURBS is probably overkill for what you do. NURBS provides that fastest block processing time available... 1ms. HPCC is 2ms, SHPCC is 4ms, and look ahead is 8ms.

 

8ms can process up to 125 Blocks Per Second (BPS)

4ms can process up to 250 BPS

2ms can process up to 500 BPS

1ms can process up to 1000 BPS

(These numbers are for Fanuc 16iM Series Controls)

 

Processing speed essentially is measured by how fast a block can be processed by the control. For example you may see documentation that states that say the control is capable of say 300 IPM but that is confusing until you figure out that the average length of movement is about .040". The smaller the move, the slower the feed you'll be able to achieve unless you are able to process those blocks faster (i.e. buying optional control upgrades like SHPCC/AICC, HPCC etc...) BPT and Block size (length of move) are the main deterniming factors that have the ultimate say so over how fast the max feedrate can be.

 

SHPCC/AICC, and HPCC also do something else better than Look-Ahead... they do what's called "Block Overlapping". Which means they look ahead a certain number of blocks (8 I think) and it treats them as 1 block. This allows the machine to get smoother acc/dec which ultimately results in higher feedrated being able to be achieved.

 

HTH

[Travis_Buchanan]

Ok how can I tell which options my control has by looking at the data sheets?

[Tom Dorgan from American Precision]

Travis, If you put a code in the program that is not enabled it should give you some type of error code. Should not hurt anything to try it.

[Ryeker]

Travis,

 

I know this was touched on by Tim but please try what he mentioned and change your post to output "I & J's". I know from experience that machining using I&J's can make a huge difference.

[George_Gerhard]

Travis

you only have advanced preview control G08P1

 

Let me explain how the option codes work. If option code one equals 46 the parameter 9100 would be 01000110 the fist four digits from the left are considered the most significant decimal, and the second four are the least significant decimal. So think of the first four as the tens column, and the second four as the ones. Bit 7 would have a value of 8 bit 6 would be 4 bit 5 would be 2 and bit 4 would be 1. So you have a one in bit 6 which equls 40. And bit 2 and 1 equal one so this is 4+2=6 40+6 =46

This is how you can find if you have a certain parameter option. Next you need to know what the option parameter is for what you want.

Sorry It is illegal for me to continue, as this is the equivalent of stealing software.

 

If you are interested I can send you a email with a brief summary of what you need to do to repair this problem

 

rgds

George