Mill/Turn Verify

[McRae]

Has anyone encountered the following warning when trying to use the verify for a milling path in a lathe session using a 5axis tool path.

 

Warning

Security Access Violation

 

Why, Why, Why??

[Harryman]

Verify has never worked for me. I ignore it.

 

Can I replace the Verify button with a smiley?

 

Here's hoping that X offers more support for REAL machining centers.

[Roger Peterson]

If you turn your tru solid off it will work. There is a true solids 5 axis verify that is available from your reseller.

 

 

HTH

[Harryman]

Reseller... Who's that?

 

I mean sorry dude maybe someday I'll get around to asking you about more of this stuff.

[Harryman]

Just for fun, I tried it. It sorta worked.

 

I'll call you on this sometime, Roger.

 

Backplot works good.

 

[ 10-01-2003, 09:51 AM: Message edited by: Harryman ]

[CNCGUY]

Harryman,

before you edited your post, you mentioned a G12.1 I am just starting to do C-Axis work and trying to machine a hex. When I post the code I get many lines of code. Should I be able to get the simple G12.1. My reseller said maybe but they are to busy right now and not sure when they can do it.

 

What can I do?

[gcode]

Check out your post.

Look for the switch mi4 ( do a text search for "mi4").

You use it by adding a 1 or -1 to the MICS value 4

It doesn't work for me because g107-g112 is an

option the machine I run doesn't have, but it may work for you.

 

[ 10-01-2003, 10:17 AM: Message edited by: gcode ]

[Harryman]

R U running Mazak?

 

Do you have a Y axis?

 

G12.1 gives X and C motions with X(radial) and Y numbers. Here's some sample code.

 

(TOOL - 38 OFFSET - 38)

(FACE CONTOUR 5/8 HELICAL INSERT ENDMILL)

N300 G28 U0.

G28 W0.

M200

T3838.0008 B20** B here is next tool

G53

M250****

G0 B0.*** B axis positioning

M251****

G17

M212

G97 G0 C0.***must position C0 B 4 G12.1, think incremental

G98

M211***C axis break

G12.1

M153

S990 M203 **mill spindle

M248

***From here on just run same XYZ moves as milling

G0 X0. Y-6.5525 Z.25

Z.1 C0.

G1 Z0. F4.5

G3 X1.9906 Y-6.2428 Z-.106 R6.5525 F4.8

X6.5525 Y0. R6.5525

X0. Y6.5525 R6.5525

X-6.5525 Y0. R6.5525

X0. Y-6.5525 R6.5525

X2.0857 Y-6.2117 R6.5525

G0 Z.25

G13.1 **G12.1 Cancel

M154

Y0.

G28 U0.

G28 W0. M205

M01

 

I need to do more homework on Verify... Shut up brain, I already told them I wasn't listening to you!

[CNCGUY]

R U running Mazak? - Emco

 

Do you have a Y axis? - No

 

Book shows X & C for each point. This is what I got from Emco tech.

 

T0000 (1/2" CARBIDE 4 FLT.)

G97 S2292 M13

M52

G28 C0

G00 G40 X1.5 Z.1 C.75

Z-1.565

G12.1

G01 G41 X1.046 C.5 F.05

C0. F.032

X.5052 C-.4375

X-.5052

X-1.01 C0

X-.5052 C.4375

X.5052

X1.01 C0

C-.4 F.05

G00 G40 X2.0 Z.2

G13.1

M53

G30 U0. W0. M15

T0000

M01

[chris m]

CNCGUY

 

That looks like a 'CX Contouring Mode' deal. The regular post output of a zillion moves is replaced by the 'endpoint' coords; right? MPLFAN has support for canned conversion:

 

#mi4 = Canned conversion cycle type selection:

# Mill-

# Activates milling axis conversation canned cycles (G107 or G112).

# 1 or -1 activates the cycle, the path continues until next entry is

# zero, sign switches (1 to -1) forces g113 at null toolchnge, the

# cycle changes or the tool changes.

 

I don't know if this could be modified to output exactly the coding you need but it probably could.

 

C

[Harryman]

Looks to me like on your Emco, you replace Y with C and X stays X(diametrical).

 

I don't get the feedrate. Are you just going super slow, or is it given in deg/min? Edit: Ok Brain here pushing that slack jawed Harryman aside... Deg/min feedrate would yield larger numbers not smaller ones.

 

The default action in the post is, I think, X and C long code. Like surfacing. Check for switches and Mi4 like Gcode said.

 

Sorry Andrew, stamp this thread HIJACKED!

 

[ 10-01-2003, 11:33 AM: Message edited by: Harryman ]

[CNCGUY]

quote:

---

I don't get the feedrate. Are you just going super slow, or is it given in deg/min?

---

I'm not sure yet!! I was thinking it was ipr of the cutter. Strange since mill is usually ipm. MCAM posts deg/min.

 

All of the stuff was in the post, all I need to do was switch it on. Now I get code I can understand. Can anyone tell me if the feed rate should be ipm or what?

 

[ 10-01-2003, 12:22 PM: Message edited by: CNCGUY ]

[chris m]

CNCGUY

 

here is some sample code from one of my progs posted with MPLFAN with mi4 set to 1:

 

G20

(PROGRAM NAME - 7348132R REVB LT15M DATE=DD-MM-YY - 01-10-03 TIME=HH:MM - 12:25 )

(TOOL - 5 OFFSET - 5)

(3/8 CARBIDE 4 FL E/M)

G0 T0505

M23

G0 G54 X2.3277 Z.25

C312.828

M8

G97 S2500 M04

Z.1

G98 G1 Z-.1 F40.

X2.1839 C309.768 F399.85

G98 G3 G112

X1.3686 C-.8383 R.0938 F12.25

G98 G3 G112

X1.2576 C-.8564 R.0938

G2 X.9765 C-.9025 R.2375

G1 X-.9765

G2 X-1.2576 C-.8564 R.2375

G3 X-1.3686 C-.8383 R.0938

X-1.397 C-.8393 R.0938

G1 X-1.5824 C-.8535

X1.5468 C-.8294

X1.3615 C-.8152

G3 X1.3331 C-.8141 R.0937

X1.2221 C-.8323 R.0937

G2 X.9765 C-.8725 R.2075

G1 X-.9765

G2 X-1.2221 C-.8323 R.2075.

.

.

.

.

 

If you change the format statement to output G12.1 or whatever it is instead of G112, would this work?

 

C

[Harryman]

IPM

[CNCGUY]

Chris,

 

Thanks. That is real similar to what I get now that I turned it on. According to the emco tech. we can't radius corners with the G12.1, has to be 6 points so I dont think changing the output to G12.1 would work. What I get with the G112 is far better than the million lines of code that you dont know what its doing.

 

Also noticed the G98 so I answered my own question from pre. post

 

Thanks Again

[chris m]

CNCGUY

 

You can set the post up to output linear moves only. I don't know the right way to do it but in this example I set the ltol to 1.000 to convert arcs to lines

 

# --------------------------------------------------------------------------

# General Output Settings

# --------------------------------------------------------------------------

sub_level : 1 #Enable automatic subprogram support

breakarcs : 1 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

arcoutput : 1 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

helix_arc : 0 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

arccheck : 1 #Convert small arcs to linear, 1=ltol, 2=atol,ltol

atol : .01 #Angularity tolerance for arccheck = 2

ltol : 1.0 #Length tolerance for arccheck = 1

vtol : .0001 #System tolerance

maxfeedpm : 500 #Limit for feed in inch/min

lcc_move : .05 #Enter the move in X, Z for lathe canned cycle comp.

ltol_m : .05 #Length tolerance for arccheck = 1, metric

vtol_m : .0025 #System tolerance, metric

maxfeedpm_m : 10000 #Limit for feed in mm/min

lcc_move_m : 1.25 #Enter the move in X, Z for lathe canned cycle comp.,mm

 

 

And, as you can see, it worked:

 

G20

(PROGRAM NAME - 7348132R REVB LT15M DATE=DD-MM-YY - 01-10-03 TIME=HH:MM - 13:09 )

(TOOL - 5 OFFSET - 5)

(3/8 CARBIDE 4 FL E/M)

G0 T0505

M23

G0 G54 X2.3277 Z.25

C312.828

M8

G97 S2500 M04

Z.1

G98 G1 Z-.1 F40.

X2.1839 C309.768 F399.85

G98 G1 G112

X1.2576 C-.8564 F12.25

X.9765 C-.9025

X-.9765

X-1.2576 C-.8564

X-1.397 C-.8393

X-1.5824 C-.8535

X1.5468 C-.8294

X1.3615 C-.8152

X1.2221 C-.8323

X.9765 C-.8725

X-.9765

X-1.2221 C-.8323

X-1.3615 C-.8152

X-1.5468 C-.8294

Z.25 F500.

X-1.5824 C.8535

Z.1

Z-.1 F40.

X-1.397 C.8393 F12.25

X-1.2576 C.8564

X-.9765 C.9025

X.9765

X1.2576 C.8564

X1.397 C.8393

X1.5824 C.8535

X-1.5468 C.8294

X-1.3615 C.8152

X-1.2221 C.8323

X-.9765 C.8725

X.9765

X1.2221 C.8323

G113

X2.1241 C50.134 F610.84

X2.2681 C46.999 F409.57

G0 Z.25

M9

G28 U0. W0. H0. M55

T0500

M01

 

This is a heinous hack but I bet some of the other guys know the 'right' way

 

C

[Harryman]

Can you use cutter comp in G112?

 

That's a main reason I use G12.1 on the Mazak.

 

I can use G2/G3 with R in G12.1

 

No comp in long code, right?

[CNCGUY]

Chris

 

Sorry if I mislead you. I like the arcs rather than sharp corners so will stick with the G112.

 

The only prob now is getting M23 (chute adv.) at hex op. and M24 (chute ret.) at following op?

 

 

I do all comp in Mcam for everything (mill & lathe) that way there are fewer setup prob. with operators. Exception being I use wear on tight tol. mill parts.

 

[ 10-01-2003, 01:55 PM: Message edited by: CNCGUY ]

[chris m]

You should be able to use the canned text, just change the M code in the string select table

 

# --------------------------------------------------------------------------

# Chute M code selection

sm73 M73 #Chute retracted

sm74 M74 #Chute engaged

schute #Target for string

 

fstrsel sm73 chute schute

# --------------------------------------------------------------------------

 

to what you want

 

C