we have a fanuc Oi-MA controller. which g-codes do you need to run to enable HSM? We don't have trocordial milling in our CAM package, but it was my understanding that you don't need trocordial tool paths for HSM (but you do for hard milling). we have a 10k spindle w/ 800ipm possible feedrates. Is it as simple as a g05.1 or something like that? and then just program it with light cuts and high feedrates?

Thats Hpcc (high precision contour control) which would
be your aceleration/deceleration function. You need to
check your machine to see what specific call out your control
requires. On a 16m you call g05 p10000- (on) and g05 p0
(off). there are no canned cycles as well as many other
functions not avail. when its(g05) active. again check
your manual.

By the way what cam package are you using?
Maybe we can talk.

PEACE:D

Right now we're using bobcad. We're a small job shop running prototracks, and a brand new VMC, so we're just getting on the CAM scene. Plan is to get a more robust CAM package in a year or 2.

If we go to really high feedrates, i'm sure we'll need to goto some fancy corner controls (golf club direction changes) and make sure our chiploads stay constant (a feature not currently in bobcad). but for now, we're curious to see how fast we can go with out the more expensive CAM.

10k spindle
1200 ipm rapids
800 ipm possible feedrates
fanuc Oi-ma control w/ standard package

we cut alot of plastics (acrylic, acetal, polycarb, uhmw) and aluminums (2021, 6061 and 7075 mostly).


I've been reading the manual that came with the machine, but i'm a bit confused at the difference between the HSM mode and the Hpcc. I know the Hpcc will clamp the feedrate around arcs based on the max allowable error, but that doesn't seem to be all that fast. correct me if i'm wrong, but the HSM mode will look ahead a bunch of blocks while the Hpcc will look ahead only 1 or 2 blocks to clamp the arc feedrates...right?

Why don't e-mail me a copy of the function details.
So we can give you a good explanation.

PEACE:D

Guys, guys, guys...

Why is it so difficult to get a Fanuc control to accurately feed on contours?

ref.

nocamhere:
g05.1

hardmill:
On a 16m you call g05 p10000- (on) and g05 p0 (off).
There are no canned cycles as well as many other functions not avail. when its(g05) active.
????

Hpcc (high precision contour control)
AICC (Artificial Intellegent Contouring Control)
That's my own name for that one... Cause it is "Artifically Intelligent" (good only for linear motion, NO circular interpolation allowed).

nocamhere:
I've been reading the manual that came with the machine, but i'm a bit confused at the difference between the HSM mode and the Hpcc. I know the Hpcc will clamp the feedrate around arcs based on the max allowable error, but that doesn't seem to be all that fast. correct me if i'm wrong, but the HSM mode will look ahead a bunch of blocks while the Hpcc will look ahead only 1 or 2 blocks to clamp the arc feedrates...right?

WOW, Can Fanuc make it any easier for a guy to get confussed?
I suppose they could, but then they'd be too much like Fadal...

In pursuit of good motion control,
Scott_bob

Hi guys,

I am in a somewhat similar situation. I sort of handle the setup of the CNC for my dad's cabinet shop, but I am trying to develop the ability to mill 7075 molds for short runs to augment my own business, which involves producing RTV/urethane rapid prototypes for the toy industry.
I am currently trying to use the CNC router to do 3d contouring and am running into acc/dec problems. It's a Komo VR510 with a Fanuc 210i-M control. In theory I can run 18,000 rpm @1250 ipm (rapid & cut). I am in the process of trying to get Komo to fax me with the option list for our 210i.
I was apparently too uneducated when we were doing our shopping, but isn't that how it usually goes. They sold us G08 as "HSHP" (high speed high precision), but now I understand it is just look-ahead. The machine works excellent for cutting cabinet parts, but when I run programs generated with VisualMill, the machine will only make 15-40 ipm actual feed. This is accompanied by hundreds of unprogrammed dwells, as you may have been able to guess.
My current theory is that Komo configured the acc/dec to deal with very long, fast moves followed by right angle turns, and back up to full speed.
If I disable G08, the machine runs acceptable feeds, but I can tell some acc/dec is needed (read: rapid gouges, inaccuracy). I have been trying for some time to decipher the Fanuc Infolink CD-ROM we got with the machine, but am looking for more direction on how to tune our servos to deal with these problems.
If anyone knows of any good books on (Fanuc) servo tuning, changing acc/dec params, angular/radius feedrate clamp settings, etc., I would be very grateful. (or maybe just a good used 15i :rolleyes: )

Thanks,

Jeremy Hill
jerhill1@netzero.com:

Jeremy, I don't know if this would be the resource you would want, but there is quite a bit of educational material on the Galil website. A lot of this information is "generic" and directed at general servo system information.

Some of it you have to log in to access the downloads, but that is easy to do. I've never been heavily spammed as a result :)


www.galilmc.com

Jeremy,

That's my son's name. Is your Komo a router or a milling machine?

Either way, have you checked out this issue:
http://www.cnczone.com/showthread.php?s=&threadid=898&perpage=25&pagenumber=3

Want to test your machines BPT?

It sounds to me like you machine is not fast enough to process the data points or motion codes your program is formated in.
Are the programs big?
Are you loading the program in the machine memory?
Is the code linear (point to point) or does it have G2 & G3 codes?

There is an awsome solution for you. Are you busy enough to go for it?

Sincerely,
Scott_bob

Thanks for the link, Hu, it's info like that, that I was looking for.

Hi Scott_bob,

It's a VR510 Mach One router, 16 hp, ISO 30, 18k rpm. I wouldn't mind trying your test program, but as I said in the previous thread, it runs fine(fast, anyway) with G08 turned off. I did get Komo to fax me with our specs, and the applicable items are:

Look-ahead control (G08)
Feedrate clamp by circular radius
Bell-shaped ACC/DEC after cutting feed
Digital servos A06B series

I think I need to research the ACC/DEC params set by Komo, and tune accordingly.

As to my CAM, I use VisualMill 5.0 and RouterCim 2004. Rcim is used for panel processing. The VM programs I've run range from 7 - 30 mb. I post them with no seq. numbers and set all options to modal to reduce the file size. I am outputting linear moves 99.9 percent of the time, because our 210i only supports G17,18,19 for circular interpolation. I've tried chordal dev. from .001 to .0001. Of course, a coarser setting reduces the problem, but with the advanced ACC/DEC turned off, the control moves through the tight programs just fine. Again, I think the problem is in the params for ACC/DEC, particularly in the Automatic Corner Deceleration Function. I think the control is seeing any corner at all as one that must be clamped, and with such small line segments, it's always in ACC/DEC. I just need to study and get familiar with Fanuc param editing (kinda scary!).

Normally, with panel-processing, we DNC (the Fanuc DOMP) directly from the CAD station over a wireless LAN. That's the beauty of the i series OpenCNC control; I only keep about 3 programs resident in machine memory. In diagnosing this particular problem, though, I have been running DNC directly off of the Fanuc hard drive. Either way, I see no difference. The Ethernet is much faster than necessary for DNC purposes. I don't have enough memory to load anything close to that big directly into the Fanuc memory. I suppose I could try a small test program, just to see, but I would be willing to bet that the DNC is not the problem.

Either way, thanks for your input, and as I said, I would be interested in seeing your BPT test program.

Good Luck,


Jeremy Hill
jerhill1@netzero.com

Jeremy,

You'd think the the manual from Fanuc would give you a good example of these parameters and the effect of adjusting them. I have not seen your manual but the Fanuc manuals I have seen aren't that helpful.

Maybe a Fanuc user here on the zone can help. It's been quite here lately with the holidays and all.

I e-mailed you the BPT program to check out. Just so there is no misunderstanding, it tests your controls speed at processing the data points (linear coordinates) into motion. Not DNC or communication through put. This is the "system" refered to in the document I sent you. The CNC control's job is to process X, Y and Z data into machine motion. The faster this process is, the better, as long as it is accurate. This should be a given but, in a lot of controls out there short cuts are taken to boost speed, unfortunately at the expense of accuracy.

Like huflung says:

__________________
First you get good, then you get fast.

Sincerely,
Scott_bob

I have a Fanuc 21i with HSM function. The code enables a look ahead which prevents "over shoot" of contour at high feed rates. I feed regularly at 200 ipm using the following format:

O1
T1 M6
M8
G49 (required before HSM activation)
S10000 M3
X3.0 Y0
G5.1 Q1 ( HSM activation required before G43)
G43 H1 Z0
G1 Y-2.5 F200.0
X0 Y2.0
etc, etc
G5.1 Q0 (turns off HSM)
G0 M9
G28 G91 Z0 M5
G90 M30

Regards,
Dave

DaveML,

Thanks for the reply!

Is the G49 (Tool Length Compensation Cancel)?
Is this needed after loading T1, or can it be done at the end of the last tool?
Your example shows it at the begining of the Tool...
Will G5.1 not work without it?

What kind of material are you machining regularly above F200.?
How fast can you machine a mold steel (Rc 40)?

Best Regards,
Scott_bob

Scott_bob; DaveML,

I got a chance over the weekend to run your BPT test program. How does 8:17 run time sound? How about 3.75 max feed?.......... Phenomenal.

If the test has nothing to do with anything but BPT, how can a 15 year-old Tandy beat our Pentium? Sorry if I seem bitter, but that's more than a little depressing.

I hold out hope that this isn't exactly the whole picture, though. I am still studying which params I can change to get our machine out of what I think is perpetual ACC/DEC on programs like these.

While it would be silly to try to change the Komo to another control (it only really needs to cut out cabinet parts), I would be interested to find out how much the Numeryx system costs, as we have an older Morbidelli CNC point-to-point/router that we might be interested in resurrecting some time in the future. The current control is an ESA (?) with no hard drive (it does have a 720k floppy, though!), and it will run a max. 300 line program (no DNC available). Worthless. The machine itself moves quick though. So I got that goin' for me,.....which is nice.


Dave,

Thanks for the input; I called Fanuc for a quote on activating the AI Advance Preview Conrol (G05.1) option on our 210i. I would cost me 5 grand+travel & lodging for the tech. That's a little cost-prohibitive for me at this time, especially when I'm not exactly sure how much it would help. I would love to hear how Scott-bob's BPT test runs on your control. The program just runs the machine in a 4" circle that's actually 60,000 small line segments instead of circular interpolation.

Thanks, guys,


Jeremy Hill

Jeremy,

Wow, that is really bad on the BPT!

That is the slowest control that I've seen tested. Sorry man...
I think you're on the right track for determining if there is a parameter you can set to make it go faster. The BPT program is good for this kind of development, as there is no angular change in direction that should be decelerated by the look ahead. And it is nothing but X and Y coordinate data movements. AIAC only works on linear interpolation (as far as I know), NO G02 or G03's...

Concidering the cost of that option from Fanuc, I'd get a quote from some of the PC based Retrofit companies around. Their performance is far better than Fanuc and they don't gouge you on Options that should be included in the control.

I'll send you your data on your BPT testing...

Best Regards,
Scott_bob

To all,

I have updated the comparison charts here in HSM thread.

Anyone suprised about the Yasnak control?
I have always liked this control compared to the Fanuc.
Fanuc is good because it is an industry standard and a lot of us know how to run it.

Perhaps it's time for you to evaluate your CNC machines central nervious system?
Brain surgery for a CNC machine? Why not?

Sincerely,
Scott_bob

Hi.

At first, sorry my worse english skill. Iam Finnish.

I Own Yang Eagle SMV-1000 milling centre with Fanuc 0MD-control. Problem is feed rates in arcs(G2, G3), example:

...
G1 X250. F600.; (Feed rate is always correct with G1)
G2 Y60. R30.; (Feed rates slown down dramatically, usually under 100)
G1 X280.; (Feed rate comes back to 600)

Second problem is when milling arcs high feed rates. Simple hole milling example:

G2 Y20. R10. F100.;
G2 Y-20 R10. ;

When i check hole diameter, its correct(with slow feed rate), when i raise feed rate, hole diameter gets smaller.

Is there some parameter what i can replace to fix this problem? Or some g-code what turn on/off hsm?