Custom drill cycle info?

[BenK]

Where can I get some info on creating custom drill cycles?

[Colin Gilchrist]

Your Reseller can provide you with the MP Post Reference Guide, which has a chapter on using the custom drill cycles. How familiar are you with Post editing? Setting up a custom cycle is a fair amount of work, depending on what you need it to do. Do you want to do a custom hole-making routine, or is this for an application like probing?

[BenK]

I'm a beginner when it comes to posts, I haven't opened one up in the last 6 months. I have the post reference guide from v9 is that still the current one?

 

I want to make some custom hole-making routines to start with and work my way up to probe routines.

[Guest]

My link

 

Try searching on Custom Drill cycles, there's already a ton of info up here too

[Guest CNC Apps Guy 1]

Hey Ben, what is it you're wanting to do/add?

[BenK]

I want to create a custom bore cycle that feeds in, stops the spindle,moves .005 off the bore and rapids out so I don't have to hand edit them all the time.

[mkd]

well if your controller will handle a G76, that would do it for you.

need to specify proper direction shift for where the boring bar ends-up during the spindle orientation, but should all be specified once in the canned cycle.

 

 

 

 

 

 

first!

[huskermcdoogle]

If it is a fanuc there are machine parameters you can set for the direction to retract. Should be under canned cycles. You program it using Q0.005, or whatever value you are looking for. I always make sure my boring bars are aligned with my drive keys, not sure if I go + or - in Y on our horizontals, but it is the same across the board in our shop, and I always load the balance hole down. Whenever I set up a machine with a boring head I always check the parameters and verify it is in the same convention as the other machines. That way there is no confusion.

 

If it is a haas you can specify the vector in the program. Just look up G76 in the haas programming manual.

 

 

Good Luck.

 

Husker

[BenK]

I have mostly Fanuc controls and one Haas. The problem with the G76 is I need to be able to specify what direction to move, we have some boring bars that we need to move in X and some in Y.

[huskermcdoogle]

I have mostly Fanuc controls and one Haas. The problem with the G76 is I need to be able to specify what direction to move, we have some boring bars that we need to move in X and some in Y.

 

Can you reconfigure you bars to all go in one direction?

 

If not you could add some logic in your post to program the parameter change to modify the direction. Then for the haas you could just use the standard G76 code, but add parameters for your direction from the custom parameters table.

 

I still say get all of the bars going in the same direction...

[Guest CNC Apps Guy 1]

I have mostly Fanuc controls and one Haas. The problem with the G76 is I need to be able to specify what direction to move, we have some boring bars that we need to move in X and some in Y.

 

Can you reconfigure you bars to all go in one direction?

...

I still say get all of the bars going in the same direction...

That is safest.. all one direction. I crated this cycle because we had some clearance issues in the tool magazine so it was what we had to do. Be cautious. With that said, this is what I did;

 

I wrote a Bore Cycle for a FANUC that allowed me to control shift direction based on the cycle ;

 

In the cycle, I would give a + or a - value in the shift amount.

 

In the machine;

 

O9014(G186 BORE + X SHIFT CYCLE)

#24=#5041

#25=#5042

G90G0Z#18

G1Z[#26]F[#9]

G4X2.

M05

M19

G4X1.

G91X[#17]

G90G0Z#18

X#24Y#25

M03

M99

 

O9015(G186 BORE + Y SHIFT CYCLE)

#24=#5041

#25=#5042

G90G0Z#18

G1Z[#26]F[#9]

G4X2.

M05

M19

G4X1.

G91Y[#17]

G90G0Z#18

X#24Y#25

M03

M99

 

In the post;

 

sgm1    : "G186"      #misc #1    - no dwell
sgm1d   : "G186"      #misc #1    - with dwell
sgm2    : "G286"      #misc #1    - no dwell
sgm2d   : "G286"      #misc #1    - with dwell

 

pmisc1$          #Canned Misc #1 Cycle
     pdrlcommonb
   *initht_a, e$
     pcan1, pbld, n$, *sgdrill, pdrlxy , pfzout , pcout, pindexdrl,
       prdrlout , *shftdrl$, *feed, strcantext, e$
   *initht_a, e$
   pcom_movea

 

pmisc2$          #Canned Misc #1 Cycle
     pdrlcommonb
   *initht_a, e$
     pcan1, pbld, n$, *sgdrill, pdrlxy , pfzout , pcout, pindexdrl,
       prdrlout , *shftdrl$, *feed, strcantext, e$
   *initht_a, e$
   pcom_movea

 

pmisc1_2$        #Canned Misc #1 Cycle
     pcan1, pbld, n$, *sgdrill, pdrlxy , pfzout , pcout , pindexdrl,
       prdrlout , *shftdrl$, *feed, strcantext, e$
       initht_a, e$

 

pmisc2_2$        #Canned Misc #1 Cycle
     pcan1, pbld, n$, *sgdrill, pdrlxy , pfzout , pcout , pindexdrl,
       prdrlout , *shftdrl$, *feed, strcantext, e$
       initht_a, e$

 

[misc1]
1. "G186 - Fine Bore (X shift)"
7. ""
8. ""
9. ""
10. ""

 

[misc2]
1. "G286 - Fine Bore (Y shift)"
7. ""
8. ""
9. ""
10. ""

 

HTH

[mkd]

^^^you got the attention of the Big Gun now^^^

 

great forum!

[BenK]

Can you reconfigure you bars to all go in one direction?

 

I wish this was an option but I will get the whole "this is the way we have always done it"

 

 

I wrote a Bore Cycle for a FANUC that allowed me to control shift direction based on the cycle ;

 

 

That is awesome thanks. Hopefully I can get this put into our post.

[Mgrenier]

Can't you use G76 with I and J instead? That is what we use here for our Fanuc controls. I shifts the X and J shifts the Y.

 

HTH

[BenK]

Can't you use G76 with I and J instead? That is what we use here for our Fanuc controls. I shifts the X and J shifts the Y.

 

I don't see anything about I or J in the Fanuc 16/18 manual.

[Thad]

I want to create a custom bore cycle that feeds in, stops the spindle,moves .005 off the bore and rapids out so I don't have to hand edit them all the time.

 

Ben, did you ever have any luck with this? I want to do this exact thing to my post and I'm not having any luck. I tried matching James' code, but no luck. The only thing that it changed is that the new text shows up in the drill cycle type dropdown list. And I get a bunch of post errors that I have to look into.

 

It's a G88 on our control.

[Thad]

Is the V9 post guide the latest documentation?

[Thad]

Nice! The V9 post ref on the FTP is password protected.

[EX-wccprogrammer]

V9 post guide is the latest COMPLETE version. They have added updates for variable modifications up through X6, available through your reseller.