[ammfg]

If some one could help me with this script i would be very grateful.



(This is the code that i am generating)


G83 X0.201 Y0.2717 Z-1. Q0.125 R.1 F10.
X0.1863 Y0.3832
X0.2384 Y0.4498
X0.2658 Y0.3777
X0.4055 Y0.4197
X0.3992 Y0.3055
X0.2832 Y0.2571
G80
G00 G91 G28 Z0.
M01

(This is what i need)

X0.201 Y0.2717
Z.1
G83 Z-1. Q0.125 R.1 F10.
X0.1863 Y0.3832
X0.2384 Y0.4498
X0.2658 Y0.3777
X0.4055 Y0.4197
X0.3992 Y0.3055
X0.2832 Y0.2571
G80
G00 G91 G28 Z0.
M01





This is my script

'G73 G83 HAAS VF Peck drilling cycle

NCEdit Output,Line = i

dim R as string
dim F as string
dim Q as double
dim Z as string

Ask Header="Pecking Parameters",Output,Cancel=canc, "Hole Depth Z"=Z, "Peck amount Q;0"=Q, "Return R"=R, "Plunge Feed F"=F

If canc Then
Exit
End If

Generate

NCEdit Line = i,Output,Text=txt

pos = InStr(txt, "Z")

If pos > 0 Then
txt = left(txt, pos - 1)
End If

txt = txt+" Z"+Z+" Q"+Q+" R"+R+" F"+F
NCEdit Line = i,Text=txt, Output, NumLines=nl
NCEdit Line = nl+1

Window2


Attachment is my cycle


If anyone can help that would be great.

[ammfg]

Cycle Menu




NC lines first point:


G83@c


NC lines intermediate point:

@c



NC lines last point:

@c
G80
G00 G91 G28 Z0.
M01





NC lines for one point:

G83@c
G80
G00 G91 G28 Z0.
M01

[moldmker]

Try this, but I have to ask, do you really want to send the Z home after each drill cycle? Seems unhandy if you need to drill multiple patterns.
(also you may need to change your G73 menu, as well)


Here's your script with some extra coding that strips the Z values off all the point coords.
Seems to work good but no warranties expressed or implied.
I stitched my script into yours, some of the variables could be consolidated, but it works.
Let me know if you want any further changes.
'G73 G83 HAAS VF Peck drilling cycle

NCEdit Output,Line = i

dim R as string
dim F as string
dim Q as double
dim Z as string
dim nl1 as integer
dim nl2 as integer
dim nl3 as integer

R=.1

Ask Header="Pecking Parameters",Output,Cancel=canc, "Hole Depth Z"=Z, "Peck amount Q;0"=Q, "Return R"=R, "Plunge Feed F"=F

If canc Then
Exit
End If

OptionsConfiguration Xchg = FALSE, Ychg = FALSE
NCEdit Output, NumLines=nl1
Generate
NCEdit Output, NumLines=nl2
OptionsConfiguration Xchg = TRUE, Ychg = TRUE

nl3 = nl2-nl1
nl3 = nl3-6


NCEdit Line = i, Output ,Text=txt

pos = InStr(txt, "Z")

If pos > 0 Then
txt = left(txt, pos - 1)
End If

NCEdit Line = i,Text=txt, Output, NumLines=nl

NCEdit Line = i+2, Output, Text=txt
txt = txt+" Z"+Z+" Q"+Q+" R"+R+" F"+F
NCEdit Line = i+2,Text=txt, Output, NumLines=nl

For v = 1 To nl3
NCEdit Line = i+v+2,Output,Text=txt
pos = InStr(txt, "Z")
If pos > 0 Then
txt = left(txt, pos - 1)
End If
NCEdit Line = i+v+2,Text=txt, Output, NumLines=nl
Next v

NCEdit Line = i+nl3+6


Window2

[ammfg]

moldmker you are the man. Thank you very much. It worked perfect


If you are asking about the G00 G91 G28 Z0. That is tool change pos. on this machine.