Camsoft and Bobcad ???

[nelZ]

Howdy!

I have version 19 Bobcad and a machine with Camsoft control. I got the post processor from Bobcad for Camsoft, it's installed.

It's iffy in that - I'm trying to do a G83 peck cycle and it does not always bring up the dialog box asking for the pecking parameters. After I select the G83 from the cycle dropdown it just generates the code without the other (necessary) parameters...

Anybody have a similar problem, OR is there another post processor which might work better for Camsoft?

Thank You

nelZ

[Karl_T]

By pure coincidence, I spent the morning writing a fanuc compatible G83 code for Camsoft pro. I'm doing all of G81 to G86 this week. My goal is to have them 100% compatible with the mastercam 6M fanuc post.

it depends on where you're an expert, you'll have either edit your post or camsoft gcodes to make them 100% compatible. I find it easier, and better in the long run, to edit camsoft

Karl

[machinationus]

Originally Posted by nelZ Howdy! I have version 19 Bobcad and a machine with Camsoft control. I got the post processor from Bobcad for Camsoft, it's installed. It's iffy in that - I'm trying to do a G83 peck cycle and it does not always bring up the dialog box asking for the pecking parameters. After I select the G83 from the cycle dropdown it just generates the code without the other (necessary) parameters... Anybody have a similar problem, OR is there another post processor which might work better for Camsoft? Thank You nelZ

You may have to modify the BobCad script file :

From BobCad Ver. 21 not sure if it works in Ver.19

'G83 ISO Peck drilling cycle

OptionsConfiguration Rel = FALSE
OptionsUnits Output, Unit = UN

NCEdit Output,Line = i

dim R as string
dim F as Single
dim Q as string
dim DEPTH as Single
dim MODE as integer

Dim FLAT as Single
Dim ANG as Single
Dim DIA as Single
dim CCS as Single
dim FPR as Single
dim RPM as integer

MODE = 98
R = .1
F = 0
DEPTH = (-1.*UN)
RPM = 0
Q = .05
DIA = .500
ANG = 118
FLAT = .010
FD = -0.00


Ask Header="G83 PECK Drill Full Depth Speed Calculator (1 of 3)", Output, Cancel=canc, "Drill Diameter;0"=DIA, "Included Angle (up to 179.99);0"=ANG, "Tip Diameter;0"=FLAT
if canc Then
Exit
Endif

CCS = 100 ' cutting speed
FPR = .003 ' Feed per rev.

Ask Header="G83 PECK Drill Full Depth (2 of 3)",Output,Cancel=canc,"Constant Cutting Speed;0"=CCS, "or RPM (overrides above);0"=RPM, "Feed Per Rev.;0"=FPR,"Plunge Feed (Overrides above);0"=F
If canc Then
Exit
End If

If CCS = 0 Then
CCS = 1
End If

If F = 0 And FPR = 0 Then
F=.001
End If

If F>0 Then
FPR=0
End If

If RPM > 1 Then
RPM = RPM
Else
RPM = CCS * 3.8 / DIA
End IF

If F<=0 Then
F = RPM*FPR
End If

Ask Header="G83 PECK Drill (3 of 3)",Output,Cancel=canc,"Full dia. Hole Depth"=DEPTH, "Retract Height"=R, "Peck amount"=Q, "Return Mode;0"=MODE
If canc Then
Exit
End If

If MODE < 98 Then
MODE = 98
End If
If MODE > 99 Then
MODE = 99
End If

FD = DEPTH

If ANG > 179.999999 Then
Exit
Endif


dim T as Single
dim K as Single
dim DEPTH2 as Single

Pi = 3.1416
T = DIA - FLAT
T = T/2
K = 90. - (ANG / 2)

M = TAN((K) * Pi / 180) * T
FD = FD + M
M = M - M - M 'neg number
'Ask Header="Drill Point Calculator",Output,Cancel=canc,"Point Depth=;0"=M, "Full Depth;0"=FD

DEPTH = (DEPTH/UN) 'some thing bobcad did wrong!
DEPTH2 = DEPTH
DEPTH = DEPTH + M ' full depth



NCEdit Line = i,Output,Text=txt
txt = "S"+RPM
NCEdit Line = i,Text=txt, Output, NumLines=nl
NCEdit Line = nl+2


Generate

NCEdit Line = i+1,Output,Text=txt
pos = InStr(txt, "Z")
If pos > 0 Then
txt = left(txt, pos - 1)
End If

txt = "G"+MODE+txt+"Z"+DEPTH+" R"+R+" Q"+Q+" F"+F+" ("+DEPTH2+" DEEP)"

NCEdit Line = i+1,Text=txt, Output, NumLines=nl
NCEdit Line = nl+1

Window2
--------------------------