MCX lathe post help wanted. Wrong CSS to RPM at end of tool.

[DavidSV]

I am having a problem. If I run CSS on a part Mastercam out puts the wrong RPM before it goes back for a tool change. Its setup to go from CSS to RPM before the change so the spindle won't slow way down and then speed back up. The problem is that MCX seems to put in the same RPM at the beginning and the end of the tool. See below. It never properly calculates the rpm before the tool change, but it calculates it right at the beginning of the tool. Is there any way to update my post to have it actually calculate the proper rpm at the end of the tool?

 

 

N2 T0202

G97 S3000 M03

G00 X.174 Z.0131 M09

G50 S3000

G96 S325

G01 X.2093 Z-.0046 F0.003

X.2393 Z-.0196

G03 X.2485 Z-.0307 R.0156

G01 Z-1.3556

G02 X.2773 Z-1.37 R.0144

G01 X.4587

G03 X.4808 Z-1.3746 R.0156

G01 X.5262 Z-1.3973

X.5616 Z-1.3796

G97 S3000 <---- 3.82*325/.5616 should be 2211rpm

G00 X6. Z6.

M01

N3 T0303

G97 S2343 M03

G00 X.5707 Z-2.08 M08

G50 S3000

G96 S350

G01 X.4144 F0.003

G00 X.5707

Z-2.0281

G01 X.4709 Z-2.078

X-.0156

G00 X.7

M09

G97 S2343 <---- 3.82*350/.7 should be 1910 RPM

G00 X6. Z6.

 

 

Has anyone else noticed this or if someone has a fix can you tell me what and where I need to change the post?

 

Thanks

[Allan]

The posts are not normally set-up like what you are talking about. Most likely the post writer has captured the inital calculated G97 speed, and is simply outputing that value before the retract. I've been asked to actually do away with the inital G97 call and just go to G96 many times, there is a switch in some post files for that now. The diffrences that you have in your speed values are quite small, does it actually cause a problem? It is possible to re-calculate the RPM value, have eyou asked your dealer?

 

Allan

[DavidB]

The speed call where you have put your comments "should be" is actually OK, if you look after your tool change the new speed for that tool is called. Its only reposting the programed speed before going to tool change position.

 

Have a look in the post and remove the spindle speed from the retract section.

[Allan]

You will want to make a call to a post block like this on the retract moves:

code:

---

 pspindle        #Spindle speed calculations for RPM

if maxss$ = zero | maxss$ > max_speed, maxss$ = max_speed

 

if css_actv$,

[

#Spindle speed calculations for strt_spd w/CSS

speedx = abs(xa)

if opcode$ = 104, speedx = abs(c1_x_min)

if opcode$ = 105, speedx = abs(tcr$)

if speedx < 0.001,speedx = 0.001

speedrpm = (conversion * g_speed) / (pi$ * speedx * two)

]

else, speedrpm = g_speed

#zero indicates spindle off (not a mistake)

if speedrpm,

[

if speedrpm > maxss$, speedrpm = maxss$

if speedrpm < min_speed, speedrpm = min_speed

]

#Spindle speed for RPM with lathe drill, thread

if opcode$ = 104 | opcode$ = 105, css_actv$ = zero

if css_actv$ = zero, g_speed = speedrpm

---

HTH

 

Allan

[monty]

quote

-------------------------------------------------

It is possible to re-calculate the RPM value

-------------------------------------------------

 

Hi Allen,

how can we recalculate it as in one of my okuma posts it outputs only 1/5th of the actual G97 value.

 

G97 S318 M03 M42 M9 ltlchg$ p__4:1475 458.

G95 ltlchg$ p__2:1453 458.

G0 X32.21 Z-58.402 ltlchg$ p__2:1453 458.

G50 S3000 ltlchg$ pcssg50 458.

G96 S200 ltlchg$ pcss 458.

G1 X30.21 F.12 llin$ plinlout 460.

G18 G3 X29.349 Z-59.441 I-1.47 lcir$ pcirlout 462.

G1 X28.178 Z-60.027 llin$ plinlout 464.

Z-64.941 llin$ plinlout 466.

X29.349 Z-65.527 llin$ plinlout 468.

G18 G3 X30.21 Z-66.566 I-1.04 K-1.04 lcir$ pcirlout 470.

G1 X31.624 Z-65.859

[DavidSV]

Thanks Allan. After looking through my post, I saw that I needed to call the pspindle command in the retract block to recalculate the RPM on the retract. Now it properly outputs the RPM before the tool change and at the end of the file.

 

David

[Godoi_Godoi]

On 1/25/2007 at 10:27 AM, DavidSV said:

Thanks Allan. After looking through my post, I saw that I needed to call the pspindle command in the retract block to recalculate the RPM on the retract. Now it properly outputs the RPM before the tool change and at the end of the file.

 

David

Hi David 

How have been ?

 

I saw the issue that you got a long time ago with G97 RPM.

I made my owm program layout in my MCX 2019 lathe pos processor,  but I'm still having  a similiar problem like yours.

Could you please tell me  What did you to solver ?

 

My problem is :

The G97 doesn't  hide when I select  CSS,  with mean The G97 is plotted  by post processor above G96 and G92.

%_N_LATHE_OP_MPF
N0 ;$PATH/_N_MPF_DIR
N10 G291
N20 G21 G40 G95 G90
N30 G54
N40 G28 U0. W0.
N50 T0101
N60 G97 S3600 M03
N70 G96 S250 M03
N80 G92 S3600
N90 G0 X0. Z0.
N100 G1 Z-10. F.25
N110 X8.842
N120 G3 X20.442 Z-15.8 K-5.8
N130 G1 Z-22.629
N140 G2 X28.842 Z-26.829 I4.2
N150 G1 X34.803
N160 G3 X46.403 Z-32.63 K-5.8
N170 G1 Z-55.347

Do you know where could I switch off the G97 when I select CCS at Post processor ?

but I don't want to delete because if I use RPM It must be released  post processor as exactlly bellow.

 

%_N_TORNEAMENTO_MPF
N0 ;$PATH/_N_MPF_DIR
N10 G291
N20 G21 G40 G95 G90
N30 G54
N40 G28 U0. W0.
N50 T0101
N60 G97 S250 M03
N70 G0 X0. Z0.
N80 G1 Z-10. F.25
N90 M30
%

 

Thank you very much....!!

Cheers..

 

 

 

 

 

 

 

 

 

[crazy^millman]

14 years later you need to provide a Z2G for someone to assist you. 

[cncappsjames]

Google doing the DEEEEEEEP Web Crawl on pre-2010 topics.

We need to dig up the very 1st technical posting and answer it as though it were asked today.