Fanuc HPCC (high speed) mode

[BrandonH]

Is it possibe to have the post processor output the high speed command (G05P1000R10)...on, (G05P0)...off, using a swich/button in the toolpath parameters page? I don't want it to come on every tool change. Just fot the 2d high speed toolpaths. I want it to be OFF by default, then ON with a check box.

 

I am using a barely modified genaric 4 axis fanuc post.

 

Current code...

 

 

( MAKINO A71 HMC )

( PROFILE ROUGH )

N220 T9 M6

N230 G0 G90 X2.1595 Y5.7506 S3565 M3

N240 G43 H9 Z3.3874 M7 T54

N250 Z2.4074

N260 G1 Z2.3676 F70.

N270 X2.027 Y5.618 F71.

N280 G3 X2.005 Y5.565 R.075

N290 G1 Y.06

------

N2610 X2.0394 Y5.3063 Z.9557

N2620 Y5.3062 Z.9582

N2630 Z.9606

N2640 G0 Z3.3874

N2650 M5

N2660 G91 G28 Z0. M09

N2670 M01

 

 

Would like it to be...

( MAKINO A71 HMC )

( PROFILE ROUGH )

N220 T9 M6

N230 G0 G90 X2.1595 Y5.7506 S3565 M3

N240 G43 H9 Z3.3874 M7 T54

N241 G05 P1000 R10

N250 Z2.4074

N260 G1 Z2.3676 F70.

N270 X2.027 Y5.618 F71.

N280 G3 X2.005 Y5.565 R.075

N290 G1 Y.06

------

N2610 X2.0394 Y5.3063 Z.9557

N2620 Y5.3062 Z.9582

N2630 Z.9606

N2640 G0 Z3.3874

N2645 G05 P0

N2650 M5

N2660 G91 G28 Z0. M09

N2670 M01

[mchin-pilot]

Misc Integers can do it.

Ask your post guy to do for you.

[Guest CNC Apps Guy 1]

You're missing out on performance by not having it on whenever possible.

 

JM2C

[Tony35]

quote:

---

You're missing out on performance by not having it on whenever possible.

---

+100

[Cannon]

We have Mpmaster post and it works great with HPCC. Off in drilling toolpaths and ALWAYS on in other toolpaths, like it should be.

[Mike Mattera - TFM]

The easiest way would be to hard code it into the start of file (psof) and the Tool change (ptlchg), to be on all the time.

 

Then in the drilling section you can put in the code to turn it off.

 

As much as I dislike hard coding things into the post, I think this one would be OK.

 

Another alternative would be to put something at the Tool change section that checks for drill and either turns if on or off. Something like....

 

if opcode = 3 # opcode 3 is for drilling

[

pbld, n$, "enter off code here", e$

]

else, pbld, n$, "G05 P1000 R10", e$

 

This should be close (it's late, I'm tired)

 

Mike Mattera

[KRESIMIR]

phpccon # Turn HPCC on

if not(hpcc),

[

if mi7$=1, n$, "G05 P10000 R10 (HPCC-ON)", e$

if mi7$=1, hpcc = yes$

]

 

phpccoff # Turn HPCC off

if (hpcc),

[

if mi7$=1, n$, "G05 P0 (HPCC-OFF)", e$

if mi7$=1, hpcc = no$

]

 

psof$ # Start of file for non-zero tool number

.

.

.

.

phpccon

.

.

.

 

ptlchg$ # Tool change

if prv_t$ = t$, [

prv_tloffno = tloffno$

tloffno$ = -1

!tloffno$

]

pinit

op_id_last = op_id$

gcode$ = 0

prv_coolant$ = 0

if coolant$, n$, "M9", e$

phpccoff

n$, "G91 G28 Z0 M5",e$

n$, *t$, "M6", ptoolcomment

#if opcode <> 16 | drillcyc <> 107, n, *ss, *spdlon

if opcode$ = 16, [

if drillcyc$ <> 107, n$, *ss$, *spdlon, e$

]

else, [

if drillcyc$ <> 7, n$, *ss$, *spdlon, e$

]

n$, *sgplane, sg00, "G90", sgwcs, "X0 Y0", "M8",e$

pcomment2,e$

n$, ptllncomp, *rapidpl,e$

protary

#if nextop = 11, ex

if opcode$ = 3,

[

n$, psg00, *xr$, *yr$, e$

#n, ptllncomp, *zr, smcool

if drillcyc$ <> 7, n$, *zr$, smcool, e$

ex$

]

 

phpccon

if zr$ < rapidpl, n$, *zr$, smcool,e$

else, !zr$, `smcool, e$

rotaxis_last = 0

tloffno$ = prv_tloffno

 

 

peof$ # End of file for non-zero tool

.

.

.

.

phpccoff

.

.

.

.

[BrandonH]

"We have Mpmaster post and it works great with HPCC. Off in drilling toolpaths and ALWAYS on in other toolpaths, like it should be."

 

This sounds like what I should be doing. My post editing is limited to adding lines for coolant cancel. Is this something I should try to tackle myself? I would like to better understand this post stuff.

 

Thank-you all for your input so far.

[Surface]

I simply do not understand why Fanuc has performance options which must be turned on. When was the last time someone complained their machine was running too fast or accurate.

[Cannon]

quote:

---

I simply do not understand why Fanuc has performance options which must be turned on. When was the last time someone complained their machine was running too fast or accurate.

---

Yes. These should not be part of the code but something that the control performs automatically, if you have purchased the options. This is only one thing where Fanuc has made an easy task hard to perform.

[Guest CNC Apps Guy 1]

quote:

---

I simply do not understand why Fanuc has performance options which must be turned on.

---

You said the KEY word here; OPTIONS. Not everybody has the same level of options.

 

Also, there are certain conditions where High Speed Look ahead/acc/dec would be detrimental to cutting. Perfect case in point - Rigid Tapping. That is DEFINITELY a case where you DO NOT want High Speed acc/dec parameters active. Your threads will not come out right. You want the spindle and the Z Axis absoultely synchronized. Another; MACRO calculations... you DO NOT want High Speed Look Ahead turned on when you're trying to do some math. You'll make a mess in a hurry.

 

There IS a parameter to make the High Speed on all the time. I always reccommend NOT turning this on because of the possibility of unintended/possibly catastrophic consequences.

 

IMNSHO, I do not see what the issue with setting the post up to automatically handle this is. :shrug:

[Tony35]

quote:

---

MACRO calculations... you DO NOT want High Speed Look Ahead turned on when you're trying to do some math. You'll make a mess in a hurry.

---

+100

a big mess

 

quote:

---

I do not see what the issue with setting the post up to automatically handle this is

---

set the defaults with HPCC (MR1) on for all milling etc i took our makino 1 step further and added (MI3) for M250-M255

 

with the MP its there just tweak it to how you want it there are some very smart people in this forum to help you make the mods

 

JM2C

[Newbeeee™]

quote:

---

The easiest way would be to hard code it into the start of file (psof) and the Tool change (ptlchg), to be on all the time.

 

Then in the drilling section you can put in the code to turn it off.

 

As much as I dislike hard coding things into the post, I think this one would be OK.

 

Another alternative would be to put something at the Tool change section that checks for drill and either turns if on or off. Something like....

 

if opcode = 3 # opcode 3 is for drilling

[

pbld, n$, "enter off code here", e$

]

else, pbld, n$, "G05 P1000 R10", e$

 

This should be close (it's late, I'm tired)

 

Mike Mattera

---

Mike,

We have hard coded G05.1Q1 at the start of all milling tools and G05.1Q0 at the end.

We don't call it for any drilling/tapping ops and it works really well.

 

As James says, if you're machine has it as an option, use it. It reduces cycle time for us on average 6mins an hour.

[Newbeeee™]

quote:

---

There IS a parameter to make the High Speed on all the time. I always reccommend NOT turning this on because of the possibility of unintended/possibly catastrophic consequences.

---

James,

+1.

Also, just for reference, there is a parameter that automatically suspends look ahead mode when in rigid tapping.

Parameter 5203 (fanuc 0i).

[Redfire427]

On our Makino's, ( S56's & V56's ) there are 3 different modes that can be used for tolerance control ( HPCC ) or SuperGI.

We control what mode we want using misc. integers.

The 3 modes are as follows.

 

M250, M251 & M252

 

M251 is the high performance mode which lowers the accuracy of the tolerance algorithms and is primarily used for roughing. Makino says this mode is roughly 30% faster than M250 which is the standard mode.

 

M250 as I just said is the standard mode and gives the machine much more defined accel/decel values and is very accurate. Almost all finishing jobs would use this mode.

 

M252 is the ultra precision mode. This mode is said to add roughly 30% more to the cycle time, however, gives you the most resolution and tolerance control.

 

We use all 3 modes at different times depending on what we are machining, but it is used at all times.

 

We had In-House Solutions modify our post to output this code. The way we select it is by inputting a value of either 0, 1, 2 in the misc. integers field In-House created for us.

0= M250 mode

1= M251 mode

2= M252 mode