Post Help

[Karl@CP PISTONS]

Using ver 9. is there any way to have the post use the toolpath groups? What I would like to do is output some macro statements then the g-code from group #1 then output other macro statements and the g-code from all of group #2 etc...

I might need to loop depending on the number of groups in a file anywhere from 1 to maybe 6 groups. We are using a modified fanuc post with the macro statements hardcoded in.

 

Thanks

Karl

[Guest]

Karl, If I understand what your looking for, you could use a customdrill cycle to be able to get your required information into a macro call statement.

 

You say the macros themselves are hard coded so

are you looking to have something like

G65 P8001 A2.5 B4.6 R.8 F50.

to define their callout?

[Karl@CP PISTONS]

JMPARIS,

I've got the post to ask questions to output the macro call.

 

What i'm looking for is this:

 

 

G65 P8001 A2.5 B4.6 R.8 F50.

g-code form toolpath group 1

 

G65 P8001 A2.5 B4.6 R.8 F50.

g-code from toolpath group 2

 

G65 P8001 A2.5 B4.6 R.8 F50.

g-code from toolpath group 3

etc...

as many times as their are toolpath groups

 

Karl

[Karl@CP PISTONS]

anyone?

[Guest CNC Apps Guy 1]

Honestly, I'd use a Manual Entry Toolpath, but that's just me.

[Karl@CP PISTONS]

James, Thanks for the reply, but The macro statement is easy in that it needs only one varible (sp?). What I need to figure out is how to post all of group one only, then output another macro call (easy) then all of group 2 etc...

Karl

[Guest CNC Apps Guy 1]

Well, I'd have to go with John's suggestion in making a Custom Drill Cycle in that case. To use the Custom Drill Parameters, you'll have to define drl_prm1, drl_prm2, drl_prm3, etc...

 

Like So...

 

In the Drill Cycle Call Section

code:

---

sgc10    G65P8000     #custom #10  - no dwell

sgc10d G65P8000 #custom #10 - with dwell

---

code:

---

#Custom Drill Variables

drl_prm1 : 0 # Custom Drill Parameter 1

drl_prm2 : 0 # Custom Drill Parameter 2

drl_prm3 : 0 # Custom Drill Parameter 3

drl_prm4 : 0 # Custom Drill Parameter 4

drl_prm5 : 0 # Custom Drill Parameter 5

drl_prm6 : 0 # Custom Drill Parameter 6

drl_prm7 : 0 # Custom Drill Parameter 7

drl_prm8 : 0 # Custom Drill Parameter 8

drl_prm9 : 0 # Custom Drill Parameter 9

drl_prm10 : 0 # Custom Drill Parameter 10

---

code:

---

# Custom Cycle Formatting

fmt A 2 drl_prm1 # Custom Drill Parameter 1

fmt B 2 drl_prm2 # Custom Drill Parameter 2

fmt C 2 drl_prm3 # Custom Drill Parameter 3

fmt D 2 drl_prm4 # Custom Drill Parameter 4

fmt E 2 drl_prm5 # Custom Drill Parameter 5

fmt F 2 drl_prm6 # Custom Drill Parameter 6

fmt G 2 drl_prm7 # Custom Drill Parameter 7

fmt H 2 drl_prm8 # Custom Drill Parameter 8

fmt H 2 drl_prm9 # Custom Drill Parameter 9

fmt I 2 drl_prm10 # Custom Drill Parameter 10 -

---

code:

---

pdrlcst         #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

if drillcyc = 9,

[

"(*** BEGIN CUSTOM CYCLE ***)", e

pdrlcommonb

"(YADDA-YADDA-YADDA)", e

n, *sgdrill, *drl_prm1, *drl_prm2, *drl_prm3, *drl_prm4, *drl_prm5, *drl_prm6, *drl_prm7, *drl_prm8, *drl_prm9, e

]

pcom_movea

---

and in the Text File,

 

code:

---

[drill cycle 10]

1. "My Custom Cycle"

2. ""

3. ""

4. ""

5. ""

6. ""

7. ""

8. ""

9. ""

10. ""

11. ""

---

code:

---

[drill cycle descriptions]

1. "G81/G82 - Drill/Counterbore"

2. "G83 - Peck Drill"

3. "G73 - Chip Break"

4. "G84 Rigid Peck Tap"

5. "G85/G89 - Bore (feed out)"

6. "G86 - Bore (stop, rapid out)"

7. "G76 - Fine Bore (shift)"

8. "Misc #2 Drill"

9. "Subprogram Call"

10. "My Custom Cycle"

11. "Custom drill cycle #11"

12. "Custom drill cycle #12"

13. "Custom drill cycle #13"

14. "Custom drill cycle #14"

15. "Custom drill cycle #15"

16. "Custom drill cycle #16"

17. "Custom drill cycle #17"

18. "Custom drill cycle #18"

19. "Custom drill cycle #19"

20. "Custom drill cycle #20"

---

code:

---

[drill custom param 10]

1. "drl_prm1"

2. "drl_prm2"

3. "drl_prm3"

4. "drl_prm4"

5. "drl_prm5"

6. "drl_prm6"

7. "drl_prm7"

8. "drl_prm8"

9. "drl_prm9"

10. "drl_prm10"

11. "My Custom Cycle Parameters"

---

Pretty much cut and paste this stuff in and modify to your liking.

 

HTH

[Karl@CP PISTONS]

Thanks Guys Great Info on the custom drill cycles.

 

Problem I have though is each part has from 1 to 6 operation groups in the operation manager.

I need the output to look like this:

 

G65 P9001 RXXXX ( R is input as a answer to a post question ) ; I got this to work

 

can't get this to work!!!

only g-code from all of tool path group #1

( end of toolpath group #1 )

 

G65 P9002 Rxxxx ( Same as R above ) ;

 

only g-code from all of tool path group #2

 

( end of toolpath group #2 )

...

...

...

end of program

 

 

Karl

 

[ 12-07-2005, 12:55 AM: Message edited by: Karl@CP PISTONS ]

[Guest CNC Apps Guy 1]

There are a number of possibilities...

 

Change the Drill statement to be only G65, then drl_prm1 to be the last digit(s), then in the drill call make like this;

 

code:

---

n, *sgdrill, "P900", *drl_prm1, *drl_prm2, *drl_prm3, *drl_prm4, *drl_prm5, *drl_prm6, *drl_prm7, *drl_prm8, *drl_prm9, e	

---

code:

---

fmt  " "  2   drl_prm1    # Custom Drill Parameter 1

---

HTH

[Karl@CP PISTONS]

James,

It must be past my bedtime 'cause I can't explain my problem clearly.

I have the macro call working...

I can't post the operation manager groups seperatly.

 

 

On a side note I think you did some work for my ex-boss a few years back (Alan Budnik). Small World Huh?

Karl

[Guest CNC Apps Guy 1]

Yes I did do quite a bit of work for him. and cool work it was.

 

I think I see now. Each group needs to have it's own NCI destination. You'll need ot go into Screen Configure, in the NC Settings Tab, click the NCI Button (I think) and have it follow the name of the "Group Name".

 

I believe thi s willl accomplish your goal.

 

HTH

[Karl@CP PISTONS]

Thanks James,

Of course now that i'm at work i'm to busy to try

this. Will try as soon as I have time (lunch or home!).

Karl