High Speed Machining not an option on my VMC

[jackmasterx3]

High Speed Machining not an option on my VMC with Fanuc OM control. Trochoidal milling can be achieved but not perfected. The dimensions that I program are not accurate to what's actually machined. I've learned that when I machine a simple counter bore, the feed rate cannot exceed 20 IPM or the tool cuts .03 undersize.

 

My question is: Does the machine have to have the "High Speed Option" to perform machining ballet or is there another way?

 

Thanks, any input would be appreciated!

[gms1]

The machine doesn't need high speed option, it just needs to cut right. If you have problems with making arcs it sounds like a machine problem. Slop in the bearings, backlash... any number of things would cause that to happen.

[Guest CNC Apps Guy 1]

Not necessarrily so gms1. Depending on the speed of cuts, machines can and do cut over/undersize. I've done testing and seen this. Corners will get blown or cut off because the servos are not keeping up with the code.

 

Jackmaster, your only remedies are to slow the feedrates down or get the High Speed Look Ahead Options for your machine.

[jackmasterx3]

Thanks CNC Apps Guy 1,

is there any other alternatives?

[Ocean Lacky™]

program for oversize holes?

[Roger Peterson]

try using the high feed function within mastercam, it won't let you cut a circle any faster, but it will let you cut fast when you can and slow down when you cannot.

 

 

HTH

[DavidSV]

Jackmaster, Have you tried a G8?

[gcode]

I destroyed a high feed cutter due to this problem a while back

I was roughing a 2" hole with a 1.25 Mitsubishi

high feed using the Mastercam helixmill toolpath.

Feedrate was 105ipm.. but I mistakenly had it set to 50% for the last pass..

The tool spiraled in great, but blew up when it got to the bottom of the hole.

 

What happened???

The machine couldn't accuratley cut the hole at 105ipm.. It was cutting .100 per wall undersized

as it spiraled in.

When it go to the bottom of the hole the feedrate

changed to 52.5ipm. The machine slowed down and

accurately finished the last pass.

Since there was .10 too much stock on the walls,

the results were not pretty

 

All the computer driven eyecandy in the world can't save you from something like that..

This is a lesson from the School of Hard Knocks

[Guest CNC Apps Guy 1]

What kind fo machine and what kind of control is it?

[Newbeeee™]

If you want to see what spec of control you actually have, and if you feel you are up to tuning the parameters, this link will help.

BUT, don't go playing if you're in any doubt.

 

http://www.practicalmachinist.com/vb/showt...9.html?t=171099

 

HTH

[mig]

What about hpcc option on control .

Look for parameters setting of acceleration and deceleration

[jackmasterx3]

CNC Apps Guy 1

 

It's a Viper V-850 VMC, 10 HP, Fanuc O-MD control, Mfg. 2002.

 

DavidSV

 

G8? Tell me more.

 

Thanks!

[Guest CNC Apps Guy 1]

Newbee, in order for those parameters to work, you HAVE to have the look ahead options (G5.1/G8) AND have them active.

 

The main poster wanted to use G8 as "it was easier" to use. Sorry but gonna have to wave the flag. If your post processor is configured properly there's nothing to think about so "easier" is NOT better in this case.

 

G8 was pretty much designed for use with prismatic type parts ONLY. It has limited look ahead capability and it has limited block processing speed (BPT).

 

G5.1Q1 (AI-NANO I)was designed for 3D and Prismatic type parts. Not hardcore sculpturing but it processes at around 2x faster than the BPT of G8 and gives you WAY more control over acc/dec.

 

G5.1Q1 (AI-NANO II) was designed for more hardcore surfacing applications but does benefit even prismatic parts. It is 2x faster than AI-NANO I in BPT and looks further ahead.

 

G5P10000 with RISC and 1,000 Block Look Ahead is the fastest and is my preferred option. Though it's not always absolutely necessary, overkill on control options NEVER hurts.

 

Depending on the control, your options for control options is limited. The 0i control will NEVER perform like a 16i, 18i, 30i, 31i or 32i no matter who you have come and tune it. About the fastest you'll get it to perform with be about 4ms BPT IIRC. It's a 486 in a Pentium World. It will get the job done but it's going ot take time.

 

Jackmaster,

To see if your machine has G8, go to MDI mode and type in G8P1; and cycle start. If you don't get an alarm, you have that option. If it does not alarm, type in G8P0; and cycle start to cancel it. Next, try typing G5.1Q1; and cycle start. If it does not alarm, type in G91; G49; G5.1Q0; G90; cycle start to chancel it.

 

HTH

 

[ 06-02-2009, 04:34 PM: Message edited by: CNC Apps Guy 1 ]

[Newbeeee™]

Oops, My Bad as they say.

I read the original post as an OiM control, in which case the link would have been helpful IF G05.1 (or G08) was installed.

I was told that G05.1 is standard on all OiM's, as it's the 'off the shelf' package from Fanuc?

But, the G05.1 has 2x parts, lookahead only (standard), and contour control (option as the link says).

 

James, you are quite correct ref MDI and seeing if the control has G8 or G5.

If the machine doesn't have either, you could still tune the acc/dec parameters to contour more accurately.

We did our leadwell (Fanuc 21M) quite successfully. As standard, it only fed accurately at F1000, any more than that and it cut corners.

After we tuned it, it contoured accurately at F2500 (although could obviously rough faster).

This was in standard (non G08) mode, as the machine had the option but the parameters were not set.

I have a spread sheet of the 1400 (feed) before and after parameters if it would help?

[Guest CNC Apps Guy 1]

quote:

---

I was told that G05.1 is standard on all OiM's, as it's the 'off the shelf' package from Fanuc?

---

Think of FANUC as a smorgasbord or Buffet if you will... When an MTB buys a control, they decide what control they want. Then they add the features that they want. NOTHING is a "standard" option as they are all added to the price the MTB pays for the control. Now with that said, there are certain things that every machine comes with, Basic Work Offsets, Tool Offsets, Canned Cycles, some method of communication be it RS-232, or Flash Card, etc... More often than not controls come with other options but what one MTB calls a "standard feature" may not be a "standard feature" on another MTB's machine.

 

Hope that clears that up.

 

You can tune the servos to improve performance without a doubt but that still won't change the amount of processing power. That requires the options. Tuning won't change the number of blocks it looks ahead and it won't change the speed at which it processes (8ms to .4ms) either.

[Newbeeee™]

James,

I think if you're doing mold type work or machining with lots of small moves in your code, then the processor speed is very noticeable.

If you're doing prismatic type parts, then not so.

Parameter tuning really helped on our leadwell, to the extent that it way outperformed the previous hitachi's where I worked, and these were all 16 controls. They would only accurately contour at F1000.

I guess its a case that some MTB's set up their machines, and some don't.

 

For the work that we do (prismatics), our Oi machines are cutting at same speed/feed as our robodrill (31ia5), F7000 both on G05.1 mode.

However, the robodrill is about 5mins/hour more productive because it is so damn quick at rapids and toolchange.

[Guest CNC Apps Guy 1]

quote:

---

...the robodrill is about 5mins/hour more productive because it is so damn quick at rapids and toolchange...

---

Yeah, they sure are quick. I love those machines. For the right kind of work they just kick @$$.

[Tony35]

cnc apps guy

so you run HPCC all the time and im starting to do that too but what is the difference between G5.1 Q1 vs G5P10000

i have 2 kitamuras with fanuc 16i controls and both options and i have to use G990 Q1(2,3)F100. before G5.1 Q1 with all the fun cancel codes before it. i find it easier to use G5P10000 (HPCC) over G5.1 Q1 (AI NANO) am i missing something here or is HPCC just better

[Guest CNC Apps Guy 1]

quote:

---

what is the difference between G5.1 Q1 vs G5P10000

---

About $5k in hardware I think.

 

You have even more control over acc/dec tuning in HPCC Mode.

 

Ive done some tests where HPCC was 20% faster than AI-NANO I. AI-NANO II is almost as good as HPCC but still not quite there. If I were a moldmaker or doing Aerospace stuff with alot of data... HPCC is the only way to fly.

 

JM2C

[Tony35]

well then it is settled than HPCC it is

 

thanks cnc apps guy