New Mpmaster

[Post dept]

All,

 

Updated Mpmaster and high speed machining notes on the mpmaster page.

 

Changes include:

 

Control def uses the same tolerance for NC precision as the output format statement. We had it tighter for arcs in previous versions but that causes helix issues (Z motion of .0001). Arc checks are working fine as are currently set.

 

safe_index (mi4$) has been added to allow the user to pick the order of indexing for 4-axis machines.

 

force_output has been added to force the output of modal G codes like G94/G95 etc.

 

High speed machining support for Fanuc and Mazak controls with mr1$ and mr2$. See the notes on that page for this as well.

 

Thanks to everyone for your help and feeback on this one. Particularily James Meyette for the high speed stuff.

 

Brett

[3R!< W3NG3R]

Is there any benefit to updating an old MC9 post to the new MPmaster? If so, what are they?

[Post dept]

Does your 9 post do everything you need it to do? If yes, then don't bother. This just has some basic new functionality and fits in a little better with the machine and control def.

[3R!< W3NG3R]

It does work fine. But what is the High speed stuff about?

[Post dept]

Post is supporting control high speed mode functionality. Look at the .doc file on the mpmaster X2 page for more info.

[3R!< W3NG3R]

Thanks Brett

[romer]

Brett,

 

Perhaps I am missing something, but one thing I noticed in the High speed functions, there is no string select definition for G49.

 

Defining it in the Misc gcode strings section works fine.

 

I liked your hsm function definitions, MUCH more elegant than the way I cobbed it out.

 

Keep up the excellent work,

 

Romer

 

P.S. The date shown for the latest update on the X2 post web page is a bit behind.

[New Job]

Did these changes apply to all mpmaster.pst's?

[Ocean Lacky™]

Need to tweak it just a little....

 

code:

---

(POST DEV  - IN-HOUSE SOLUTIONS)

(T11 - 1 INCH BALL ENDMILL - H11 - D11 - D1.0000" - R0.5000")

(T3 - 1/2 BALL ENDMILL - H3 - D3 - D0.5000" - R0.2500")

(OVERALL MAX - Z2.)

(OVERALL MIN - Z-1.9984)

G00 G17 G20 G40 G80 G90

T11 M06 ( 1 INCH BALL ENDMILL)

(MAX - Z2.)

(MIN - Z-1.8285)

(TOOLPATH - HMM)

(STOCK LEFT ON WALLS = .03)

(STOCK LEFT ON FLOORS = .03)

G00 G90 G54 X-.0451 Y-.06 S3000 M03

G43 H11 Z2. T3

G94

G61.1 ,K30

G05 P2

M50 <==(Turn Air On)==Need to move before G61.1

Z.483

G01 Z.233 F75.

X-.0449 Y-.0596 Z.2252

X-.0441 Y-.0586 Z.2174

X-.0429 Y-.057 Z.2098

---

And....

 

code:

---

X.1856 Y.5979 Z-1.7835

X.183 Y.5988 Z-1.7763

X.1812 Y.5994 Z-1.7688

X.18 Y.5997 Z-1.7612

X.1797 Y.5998 Z-1.7535

Z-1.6662

Z-1.5285

G00 Z2. <=====Need to move after G64

G05 P0

G64

M09

M05 <==(Turn Air On)==Need to move before G61.1

G91 G28 Z0.

M01

T3 M06 ( 1/2 BALL ENDMILL)

(MAX - Z2.)

(MIN - Z-1.9984)

(TOOLPATH - HMM)

(STOCK LEFT ON WALLS = 0.)

(STOCK LEFT ON FLOORS = 0.)

G00 G90 G54 X-.9076 Y-1.1569 S7500 M03

G43 H3 Z2. T11

G94

G61.1 ,K30

G05 P2

M50

Z.393

G01 Z.143 F50.

X-.9077 Y-1.1565 Z.1349

X-.9078 Y-1.1552 Z.127

---

These will cause Mazak's PC Fusion 640 to alarm out. Where can I make these changes?

[Roger Martin from CNC Software]

Ocean Lacky,

 

Moving the Air ("coolant") command "up" appears to be fairly simple...

 

This assumes that you are using the ‘X’ style coolants to add the M50 (Air) command.

With this ‘coolant’ command activated in the toolpath parameters in the ‘after’ mode.

 

Adding a call to pcan2 call here in ptlchg_com->

code:

---

ptlchg_com      #Tool change common blocks

 

... snipped lots 'o code ...

 

phsm1_on #must remain before G43

pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$

pcan2 # <ADDED>

phsm2_on #must remain after G43

---

Results in this tool startup code sequence ->

 

N140 G00 G90 G54 X.3264 Y-.2507 S2139 M03

N150 G43 H235 Z.25

N160 M50

N170 G94

N180 G61.1 ,K0

N190 G05 P2

N200 Z.1

N210 G01 Z-1. F6.42

 

 

As for moving the HSM mode cancellation "up above" the Z-axis retract. This is going to be a lot more involved....

And better left to the MPMASTER "masters" (aka. The capable crew @ In-House) to handle.

[Ocean Lacky™]

Thanx, Roger, that worked. I did find another quirk, though

 

 

code:

---

X-5.6129 Y7.7213 Z-.0499

Z.0751

Z.1251

G00 Z2. <=======Change to G01 Z2. (Max Feedrate)

(TOOLPATH - FINISHSCALOP)

(STOCK LEFT ON DRIVE SURFS = 0.)

X-7.4565 Y9.6629

Z.05

G01 Z0.

X-7.4679 Y9.6512 F100.

X-7.5045 Y9.6131

X-7.5135 Y9.6033

X-7.5425 Y9.5713

---

This generates an Illegal Format error.

 

 

Thanx again for the help

[Guest CNC Apps Guy 1]

I needed to tweek a little proper HSM cancellation

 

code:

---

ptlchg$          #Tool change

pcuttype

toolchng = one

toolcount = toolcount + 1

if toolcountn <= tooltotal, nexttool = rbuf(4,toolcountn)

else, nexttool = first_tool$

if wcstype = one, #Work coordinate system

[

pfbld, n$, *sg28, "X0.", "Y0.", e$

pfbld, n$, "G92", *xh$, *yh$, *zh$, e$

]

"G90", e$ # <---------- ADDED TO HAVE MACHINE TO ABSOLUTE POSITIONING MODE

"G49", e$ # <---------- ADDED TO CANCEL HSM OPTIONS PROPERLY

if mi10$=one, n$, *sm00, e$

else, pbld, n$, *sm01, e$

" ", e$

ptlchg_com

---

And Rigid Tapping with Pecking ...

 

code:

---

ptap$            #Canned Tap Cycle

pdrlcommonb

#RH/LH based on spindle direction

if use_pitch = 0,

[

"M05", e$

"M80", *speed, e$

pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout, pindexdrl,

prdrlout, *peck1$, *feed, strcantext, e$

]

else,

[

"M05", e$

"M80", *speed, e$

if met_tool$, pitch = n_tap_thds$ # Tap pitch (mm per thread)

else, pitch = 1/n_tap_thds$ # Tap pitch (inches per thread)

pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout, pindexdrl,

prdrlout, *peck1$, *pitch, !feed, strcantext, e$

]

pcom_movea

---

[Post dept]

Thanks for the feedback guys. Just got back from Westec and will look at this stuff soon.

 

Brett

[Post dept]

Ocean Lacky,

 

I've been told that the Matrix control can handle any Gcode from G0 to G3 inside G61.1. I can't find the info in the Fusion control though.

 

You need it to force high feed?

 

CNC Apps Guy,

 

Looks like the sg49 string was missed. It would be nice to keep that as part of the hsm post blocks so it's definietly modal on a restart. So I've got:

 

code:

---

 

N150 G49

N160 G94

N170 G05.1 Q1

N180 G43 H263 Z125.9772

 

---

What's the deal with the G90?

 

I'll work on updating the tapping to the 21st century next.

 

Brett