Post question

[Guest]

I am creating a specific gun drill cycle as we are doing more and more of this it makes sense for me now.

 

code:

---

pgundrill

pdrlcommonb

drill_speed = dwell$

start_hgt = peck1$

drill_feed = peck2$

pbld, *sg01, start_hgt, *feed, e$

pbld, drill_speed, e$

pcan1, pbld, n$, *sg01, pdrlxy, pfzout, *drill_feed, strcantext, e$

pbld, n$, sg00, *start_hgt, e$

 

pcom_movea

---

My start height is actually inside of the part

 

 

The cycle itself looks like this

 

code:

---

N4 T4 (438 X 9.5 IN GUN DRILL)

M6

(MAX - Z6.625)

(MIN - Z-.25)

G00 G90 G54 X-.9511 Y-3.8789 S500 M03

G43 H4 Z6.625 M88 T1

G01 Z3.885 F10.

S1500

G01 Z-.25 F1.7

G00 Z3.885

G80 M89

M05

G91 G28 Z0.

---

I am looking to be able to get a retract into the section before the G91 G28 move.

 

For obvious reasons I do not want to hardcode a height.

 

Any ideas how I can get a clearance height into here?

 

I am having a brain fart on this.

[Paul Decelles]

Why not just use the Clearance height (G43 line) and retract height (your G1 line immediately following) so you can take advantage of the absolute/incremental options with those fields in the drilling dialog? All I see there is a long hand drilling cycle, no need for anything special.

[Guest]

DUH!!!!!

 

Paul thanks.

 

Like I Said brain fart too many things on my plate

[Bpin]

John,

If I start my spindle with the drill not in the hole it becomes a fan blade just prior to shooting across the shop.. don't think this code would work for me !

 

Happy Friday

[Chris Parish]

Bpin:

 

I would normally agree..however, I have a customer that turns on the spindle about 1/2 inch deep into a previos hole... It works quite well ... I was surprised.. so I modified their post as to what they liked...

[Guest]

We've done this just like that in the past, it is the manufacturer's recommendation to turn it on about 500 RPM, then once in the hole beffore begining the feed to turn it up to the cutting RPM

 

We use Drill Masters/El Dorado Tool

[Psychomill]

John, something to keep in mind on gundrilling too....

 

I will always spin the drill backwards into the hole before turning it on. The drill you're using isn't that long on the DIA/LOC ratio so you're probably ok. But I had times with really long gundrills where the cutting edge catches the side of the pilot hole going in and crapping the drill out (and/or the part). Dropping the drill in spining backwards eliminated that.

 

[Guest]

THis drill on this part 1s .438 and it's 9.5" long 21X the diameter, not too bad

 

But on something longer that does sound like a good idea.

 

[Bpin]

I always pilot a 1.7 inch deep hole (1/4" dia)

and then feed my gun drill in 1.5 deep and guide the end in the hole by hand then 500 rpm and feed 15 ipm to .2 above previous drill then 2500 rpm and 1.3 feed to depth. My 36" and 48" long drills droop about 2 inches so you have to guide them in by hand not spinning. It's quite a reach to have left hand on drill end and right hand on feed override...

[DavidB]

John,

You might want to slow the spindle speed back down to 500 before you exit the hole to.

 

I use the same method with with drills over 16xD

[Guest]

I did David, after I "fixed" my oversight, I added that in

 

[DavidB]

John,

Where did you put your pgundrill into the post?

 

I'm using the Generic 5-axis Fanuc post

 

Thanks

[Guest]

in replaced the pdrill$ call in misc2 with pgundrill and placed the postblock pgundrill right after misc1

 

code:

---

pmisc2$          #Canned Misc #2 Cycle (User Option)

pgundrill

---

and right afetr pbore2$

 

code:

---

pgundrill

pdrlcommonb

drill_speed = dwell$

start_hgt = peck1$

drill_feed = peck2$

pbld, *sg01, start_hgt, *feed, e$

pbld, drill_speed, e$

pcan1, pbld, n$, *sg01, pdrlxy, pfzout, *drill_feed, strcantext, e$

pbld, n$, sg00, *start_hgt, e$

pbld, n$, *speed, e$

pbld, n$, sg00, clr_hght, e$

pcom_movea

---

I also changed this at the bottom of the post in the "old" text section

 

code:

---

[misc2]

1. "Gun Drill"

2. ""

3. "Drill Speed"

4. ""

5. ""

6. ""

7. "Drill Start Height"

8. "Drill Cycle Feedrate"

9. ""

10. ""

11. ""

---

and cchanges this in the drill cycle descriptions at the bottom

 

code:

---

8. "Gun Drill G01 Feed"

---

[Guest CNC Apps Guy 1]

+1 to David. I always turn on the spindle at like 250-500 RPM, move to the hole, feed down into the pilot hole (.0005-.001 larger than the hole being drilled)I created 1-2x Diameter deep, turn on the high pressure coolant, dwell 1 sec., ramp up the spindle, dwell, 2-3 sec(will vary on how long the spindle takes to ramp up), feed to the bottom, turn off the coolant, dwell 1 sec, ramp down the spindle, dwell 2-3 sec., retract out, move to the next position and repeat the process. Yeah there's a lot of dwells there but when going 30xD+ ... it's worth the time for the results I get.

[PcRobotic]

I used your post as MAKINO tap, so how do I change from G81 to G84?  Thank you.

 

 

N1(0-80 CUT TAP)
G0 G17 G40 G49 G53 G80 G90 Z0
T1 M6(, CUT#2)
G90 G54 A0.
X1.42 Y5.5891 S800 M3
G43 H1 Z1. T3 M8 M135 S800
(DOC= Z0.)
G98 G81 Z0. R.25 F10.
X1.92
X2.42
X2.92
X3.42
X3.92
X4.42
X1.92 Y6.0891
X2.42
X2.92
X3.42
X3.92
X4.42
X4.92
G80 M9
M5
G0 G17 G40 G49 G53 G80 G90 Z0
G53 Y0
M1
T3  M6
M30
%

[Guest]

That cycle is hardcoded with a G81, a gundrill cycle you don't peck

 

A G83 cycle is already available in a post, so I don't understand why you would implement this instead

[betts]

I always pilot a 1.7 inch deep hole (1/4" dia)

and then feed my gun drill in 1.5 deep and guide the end in the hole by hand then 500 rpm and feed 15 ipm to .2 above previous drill then 2500 rpm and 1.3 feed to depth. My 36" and 48" long drills droop about 2 inches so you have to guide them in by hand not spinning. It's quite a reach to have left hand on drill end and right hand on feed override... graemlins/cheers.gif

Pin what the heck are you drilling 4' deep? And how many beers does that take?

[PcRobotic]

That cycle is hardcoded with a G81, a gundrill cycle you don't peck

 

A G83 cycle is already available in a post, so I don't understand why you would implement this instead

I did it, because I want to combine MAKINO, MATSUURA, HAAS, YCM and SUPER MAX  tapping cycles into one POST.

[Guest]

lol, a frankenpost

 

At some point in time that  will  become a nightmare for someone, good luck with it

 

I have seen it before

[EX-wccprogrammer]

JParis, on 29 Oct 2014 - 1:15 PM, said:

lol, a frankenpost

 

At some point in time that  will  become a nightmare for someone, good luck with it

 

I have seen it before

 

I have a post that outputs code for Mazak, Mori-Seiki, Haas, Meldas and Fanuc.  It works very well, thank you. 

[MIL-TFP-41]

I did it, because I want to combine MAKINO, MATSUURA, HAAS, YCM and SUPER MAX  tapping cycles into one POST.

There are much easier & cleaner ways of doing this. I have Matsuura, Fanuc, Siemens, & Yasnac all in one post......using something like what EX-wccprogrammer outlines in this post:

http://www.emastercam.com/board/topic/78945-mastercam-posts/

is much cleaner, easier, & far more versatile for future upgrades.

[PcRobotic]

I have a post that outputs code for Mazak, Mori-Seiki, Haas, Meldas and Fanuc.  It works very well, thank you. 

Hi Ex-Programmer,

   Would you please share with us how you made that post with all tap codes?  Thank you.

[EX-wccprogrammer]

This is from my post.

ptap$
       pdrlcommonb
       result = newfs(17, feed)  # Set for tapping Feedrate format
       if met_tool$,
         [
         if toolismetric, pitch = n_tap_thds$  #Metric NC Code - Metric Tap
         else, pitch = (1/n_tap_thds$) * 25.4  #Metric NC Code - English Tap
         ]
       else,
         [
         if toolismetric, pitch = n_tap_thds$ * (1/25.4)  #English NC Code - Metric Tap
         else, pitch = 1/n_tap_thds$           #English NC Code - English Tap
         ]
       pitch = pitch * speed #Force Units Per Minute for regular Tap cycle
       if machinepick = 8 | machinepick = 11,
        [
         pcan1, pbld, *sgdrlref, *sgdrill, pfxout, pfyout, pfzout,
           pfrdrlout, *pitch, !feed, strcantext, "H0", *speed, e$
        ]
       if machinepick = 4, "M29", *speed, e$
       if machinepick > 8 & machinepick <= 16 & machinepick <> 11, "M29", *speed, e$
       if machinepick <> 8 & machinepick <> 11,
        [
         pbld, pcout, e$
         pcan1, pbld, *sgdrlref, *sgdrill, pfxout, pfyout, pfzout,
           pfrdrlout, *pitch, !feed, strcantext, e$
        ]
       pcom_movea

Please take note that this code is not copy paste for your post.  There is some other editing that needs to be done to make this functional.  I posted this to illustrate how I combined multiple formats into something I find very convenient.

[jeff]

in replaced the pdrill$ call in misc2 with pgundrill and placed the postblock pgundrill right after misc1

 

code:

pmisc2$          #Canned Misc #2 Cycle (User Option)      pgundrill 

 

and right afetr pbore2$

 

code:

pgundrill      pdrlcommonb      drill_speed = dwell$      start_hgt = peck1$      drill_feed = peck2$       pbld, *sg01, start_hgt, *feed, e$      pbld, drill_speed, e$      pcan1, pbld, n$, *sg01, pdrlxy, pfzout, *drill_feed, strcantext, e$      pbld, n$, sg00, *start_hgt, e$      pbld, n$, *speed, e$      pbld, n$, sg00, clr_hght, e$      pcom_movea

 

I also changed this at the bottom of the post in the "old" text section

 

code:

[misc2]1. "Gun Drill"2. ""3. "Drill Speed"4. ""5. ""6. ""7. "Drill Start Height"8. "Drill Cycle Feedrate"9. ""10. ""11. ""

 

and cchanges this in the drill cycle descriptions at the bottom

 

code:

8. "Gun Drill G01 Feed"

 

 

JP,is it safe to assume this is the finished product? I want to try and implement this into my post.

[Guest]

I've got a newer version of that...hang on