High speed milling

[and5577]

Hi,

I am presently trying to use the G05 command on a Fanuc 18i- MB control, Yes, it does work but is too slow, I was wondering if anyone out there could give me any tips on setting the parameters in the control to get it cut more efficiently.

 

Many thanks in advance.

[Salahuddin]

there was a lot of topics about the High speed, if you try the search you will find a lot of topics.

any way you have to be more clear about your problem and what you need.

like: what speeds and feeds you use now?

what machine? what type of work?

what you mean its slow? is the machine slowing down in some area or its slow all the time?

I have fanuc 18i and it have the option of SHPCC

I use it only with some kind of parts

 

and welcome to the forum

[and5577]

Thanks for the reply.

Hi have tried searching through the manuals and the internet but it seems that the more I read the more confusing it gets.

I have set the feed at 5.0 meters, which leaves rubbish definition, when I put in G05 at the start of the program it does a great job but takes 5 times longer. Surely there is a happy medium.

[Salahuddin]

what toolpath you are using? what tolerance?

which ver of mastercam?

5 time longer is not a great job for sure.

[and5577]

Hi

I am using surface finish contour with .02 mm tol

on Mastercam X4.

 

Tim

[Salahuddin]

Hi Tim

is the filtering is on?

its in the Total tolerance / line/arc filtering settings.

[and5577]

Yes it is but the tighten line or arc is not checked at the bottom of the box.

 

Tim

[mig]

G05 is not enough .

Cod must look like that

%

O0000(5120851)

(DATE=DD-MM-YY - 07-09-10 TIME=HH:MM - 13:26)

(MCX FILE - Z:SRVDRWBALLARDBALL134.877_UMD HT PLATESWORKING5120851.MCX)

(NC FILE - C:TOYODA NC5120851)

(MATERIAL - ALUMINUM INCH - 2024)

( T243 | 1 INCH FLAT ENDMILL | H243 )

G20

G0 G17 G40 G49 G80 G90

( TOYODA - AF610 )

( MACHINE GROUP-1 )

G05 P0(HPCC_OFF)

T243 M6

G0 G90 G55 X-7. Y-3.5 A0. S534 M3

G43 H243 Z.25

M602 (HPCC_Semi-Finishing)

G05 P10000(HPCC_ON)

Z.1

G1 Z0. F6.42

Y-4.5

G3 X-6. Y-5.5 I1. J0.

G1 X-5.1087

G3 X-4.1087 Y-4.5 I0. J1.

G1 Y-3.5

Z.1

G0 Z.25

M5

G05 P0(HPCC_OFF)

G0 G91 G28 Z0.

G0 G28 X0. Y0. A0.

M30

%

[MotorCityMinion]

Mig nailed it, G05 P10000 turns it on G05 P0 turns it off. You must turn it off between tool changes also. I've never seen a decrease in feed rates using the G05, perhaps neutral, but never slower.

 

Mig, M602 is foriegn to me. What does it do?

[mchin-pilot]

High Performance Cutting Condition????

[and5577]

HI Guys

 

Thanks for all your help so far.

 

I have tried all your suggestions so far with no reward, with the P10000, the control throws up an error saying improper G code but it recognises G05 Q1.

I'm thinking it must be the parameter settings in the control that is making it go so slow in the corners.

Any more help greatly received.

 

Tim

[peon]

What make machine are you operating? Does it machine faster without the G05 Q1? I have operated a Yama-Seiki machining center with an 18i controller with the same G05 Q1 code and didn't make a difference. It was just plain slow. The machine was a POS with a wonderful controller. Lipstick on a pig is still a pig. The machine installer advertised it as a high speed machining center ONLY because the controller had the high speed option.

[and5577]

Hi

 

The machine is a Mitsubishi DCH50 horizontal, it works fine without the G05 Q1, it's just that I need more cornering accuracy.

[peon]

You may want to contact the machine manufacturer and ask them for some alternative parameter settings. I'm sure they can help you with some settings for roughing and finishing.

[Cannon]

You can adjust the accuracy vs speed in AICC. If it is set in the control you should be able to adjust it by putting R1-10 at the end of the starting code. For example G05 Q1 R2. (1 is the fastest and 10 is the most accurate)

[Newbeeee™]

Sounds like the servo's need their parameters tuning.

The machine probably left the factory with a 'standard' set of values in the parameters.

Standard (non G05) machining uses one set of parameters, where lookahead (G05) uses another set.

Depending upon how confident you are, you can do this yourself in an afternoon.

[Redfire427]

Interesting. On our Makino's, there are actually 3 options for tolerance control. Like others have stated, to turn it on, the code is G5 P10000.

It is then follwed by an M-code that controls the tolerance. These modes are M250, M251, and M252

M250 is the standard tolerance mode ( accuracy around .00013" )

M251 is the high performance mode which is typically used for roughing ( accuracy around .0008"

M252 is used for ultra accuracy ( accuracy around .00008" )

 

Makino says that if you use the M250 as a benchmark, M251 will run about 30% faster and M252 will run about 30% slower. This of course depends on the geometry. After 6-1/2 years of running nothing but Makino's, I would say they are very close estimates.

 

Good luck on getting it figured out.

 

Carmen

[shazam/TPP]

same problem but with Hardinge/Bridgeport XR760 Fanuc 18i-MB has the nano tech.

[and5577]

Seem to have got the problem sorted now, thanks to you guys and a lot of trawling through Fanuc manuals. It was the perameters that were just set too slow, they still need tweeking but know where I am going now.

 

Thanks again.

 

Tim