Can I insert saftey/stop move?

[millman2002]

Hi All:

Is it possible to insert a saftey/stop move before or after a operation on the Operation Manager?

 

(saftey/stop move)

G0G80G90M5M9

Z0G53

X0Y0Z0E0H0

M0

 

This is for Fadal.

 

Like this....

 

1. pocket

2.contour

3.(insert g code)

4 contour

 

I hope you understand...

Thanks

Gary

[McRae]

Use manual entry and cut and paste the routines you need. 1005 and 1006 - post the code to find out if you have got brackets around the code or not. (If the code comes out bracketed, then the machine will ignore it as a comment so watch out!)

[Keith Graydon]

Yes,

Use "Manual Entry" tool path. Typeit in the dialog. Or Type it in a text editor and save it. You can call up that file in MAnual entry also. Pretty cool

 

HTH

-KLG

[McRae]

Kieth - Must have hit send just before you did.

 

Great Minds...

[Keith Graydon]

Heh, You just type faster good point about thos bracekts 'tho.

 

[ 10-07-2002, 10:33 AM: Message edited by: Keith Graydon ]

[Smit]

This is what I've done to my post to make it do what you're asking.

 

pstop # Stop routine

pretract

pcom_moveb

if mi10=one, n, "X0.Y10.Z0.E0H0", e

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

if mi10=one, n, ptoolcomm, e

 

On the parameters page activate the misc values box and set mi10 to 1, this will put an M0 before the operation.

When a manual entry is posted it will appear after the M0.

Note: You'll need to add a G54 (or whatever) to the code at start up, as you've canceled it with the E0.

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs,

pfxout, pfyout, pfcout, *speed, "G54",

*spindle, pgear, strcantext, e

The above is one line.

Works well for me.

Smit

[McRae]

After reading smit's post, Force tool change would do the same thing between operations. That is if the post will spit out an M1 and the optional stop is activated.

 

Smit - Very elegant solution. If you leave the E0 off the block will the Fadal retain the proper work coordinate?

[Smit]

In V9 the force tool change has a bug in it that causes a program stop each depth cut when using multiple depth cuts. It has been recommended to me not to use this feature in V9. It does work well in V8. If the E0 is not included the table will move to the work offset position of X0, Y10., Z0. (set in my post). I'm not sure what the Z will do with an H0, I've never tried it. Then it will retain the original setting. When I tried to force PWCS the post gave me an error, so I settled for the "G54". It's not ideal, and you have to be aware of it if you're using multiple work offsets, but it's liveable.

[kathy]

Smit -

 

Pretty Clever. I modified my Fadal post almost excatly the same way; using M10=1 to call the pstop sub-routine! We mostly use a pstop between two contours machined by the same tool, to change clamps. I put in a point at the begining of the second contour.

 

works like a champ

 

Kathy

[Keith Graydon]

The Standard MPFADAL2.pst has this functionality. Set Mi1 to "1" and Z will retract and the table will position out towards operator. It doesn't allow for Comments or M0. Smits solution is much nicer but this will work in a pinch. It posts with block delete on so remember to throw the "/" switch on.

 

-----read on.

------8<-----snipped ----------8<--------

[pre]

code:

---

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

# Features:

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

# This post supports Generic FADAL (FORMAT 2) code output for 3 and 4 axis milling.

# Subprograms are also supportted. Subroutines are NOT supportted.

# It is designed to support the features of Mastercam Mill V8.

#

# Following Misc. Integers are used:

#

# mi1 - Work coordinate system

# 0 = Reference return is generated and G92 with the

# X, Y and Z home positions at file head.

#

1 = Reference return is generated and G92 with the

# X, Y and Z home positions at each tool.

# 2 = WCS of E1, E2.... based on Mastercam settings (workofs).

#

# mi2 - Absolute or Incremental positioning at top level

# 0 = absolute

# 1 = incremental

#

# mi3 - Select G28 or G30 reference point return.

# 0 = G28, 1 = G30

#

---

[/pre]

 

my .02

KLG