Fadal post - force G8 for milling only

[Thad]

We're trying to modify our post to cleanup the code. Currently, we force a G8 (no feed ramps) at the beginning of every program. Then on drilling programs, we force a G9. On rigid tapping, we force a G8. The end result, while it works, is messy.

 

How can I output a G8 on only milling cycles?

 

We've got the G8 on rigid tapping and G9 on drilling cycles taken care of.

 

Thad

[Mjölnir]

quote:

---

How can I output a G8 on only milling cycles?

---

Not quite the answer you're looking for, but I use "Manual Entry" for such things. Allows me to use the same post for the Fadal Legacy controls and the Fadal 104/D where G8 has been superceeded by G8.1 for example.

[crazy^millman]

Thad look to the MPMASTER and the opcodes this gives you the flex ability you are looking for to accomplish this task. For others there is a MPMASTER_FADAL post that works very good.

 

HTH

[Psychomill]

Or you could add this.. I do something similar on posts for different reasons....

 

if tool_typ > 9, "G8", e$

else, "G9", e$

 

 

I haven't tried this in X yet. Should work as long as you're not trying to do some milling with a drill. Then just leave the G8 forced in the tap cycle. Although, if you drill with a chamfer mill (type 12), it will still output a G8....

 

[Steve Arteman]

Thad,

I'm thinking this works the same in the x post here is something I made for a Fadl post in V-9

 

 

pg8g9 #Add either G8 To Milling or G9 to drilling SLA

If opcode = 3 , "G9"

if opcode < > 3, "G8"

[Trevor Bailey]

Dont use tool_typ, use the opcode method.

[Guest CNC Apps Guy 1]

I use opcode for the HSM cycles in the machine (Look Ahead, AICC, AI NANO, HPCC, etc...). Works 100% unless you have Macro Cycles and you're driving them off Custom Drill Cycles, in which case you'd need to say someting like

 

if opcode=3 | drill_cyc > somenumber

 

Somenumber being determined how you have the cycles set up.

 

HTH

[Thad]

Thank you all for your replies. I'll have to print them off and look at them at another time. We went from nothing to do to being swamped.

 

Thad

[Psychomill]

quote:

---

Dont use tool_typ, use the opcode method.

 

---

+1 trev.... my bad...

 

[TheePres]

Exact question i was planning to ask.

Does opcode=3 signify a drilling operation?

[Guest]

Yes Theepres it does

 

From MpMaster.

 

quote:

---

sop03 "DRILL/MISC." # " "

---

[TheePres]

I see now, never noticed the sop strings till now.

[Steve Arteman]

ThreePres,

You can look in the new post for the opcodes but as James said above you can get more specific to the drill cycle using the drill_cyc if you need to.

Steve

[TheePres]

Correct me if im wrong, but seems to me that opcodes as shown in MpMaster post were intended for insering comments in NC code, making this an ingenious way of achieving this "G8-G9" result.

Is there a "more direct" Mastercam post code that differentiates between different toolpaths?