fadal g91 after tool change ?

[bthomps5]

91v-MPFADAL1-1 post always has out put g91 at end of tool instead of g90 i always just edit them is there a way to change this? thank you in advance

[Don S at Barefoot CNC South]

yes

[Guest]

Can you post your pretract section so we can see how it is being output and then we can tell you what you need to change.

 

It is likely a hardcoded "G90" but need to be sure

[bthomps5]

here we go thanx for the quick replys

 

N20( 2 INCH FACEMILL TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - 2.)

N21T2M6

N22G0G90S1400M3E1X-1.2Y1.02

N23H2Z.1

N24G1Z-.135F10.7

N25X0.F50.

N26X37.5

N27X38.7

N28G0Z.1

N29Y-2.02

N30G1Z-.135F10.7

N31X37.5F50.

N32X0.

N33X-1.2

N34G0Z.1

N35M5

N36G91H0Z0.<----want to change to g90

[Guest]

Thats' the pretract section of your post?

 

[bthomps5]

is this what you mean ?

 

 

pretract #End of tool path, toolchange

sav_absinc = absinc

absinc = one

sav_coolant = coolant

coolant = zero

#cc_pos is reset in the toolchange here

cc_pos = zero

gcode = zero

pcan

pbld, n, sccomp, *sm05, scoolant, psub_end_mny, e

pcan1, pbld, n, sgabsinc, sgcode, "H0", "Z0.", strcantext, e

# pbld, n, sgabsinc, sgcode, *sg28ref, "Z0.", scoolant, e

# pbld, n, *sg28ref, "X0.", "Y0.", protretinc, e

pcan2

absinc = sav_absinc

coolant = sav_coolant

[Guest]

Yup, that is what I meant

 

Change this line

 

code:

---

pcan1, pbld, n, sgabsinc, sgcode, "H0", "Z0.", strcantext, e

---

to this

 

code:

---

pcan1, pbld, n, sg90, "H0", "Z0.", strcantext, e

---

[bthomps5]

thanks that works great. you are very quick, you the man!

[bthomps5]

man quick response last time i asked a question any help would be appreciated change g99 out put to g98

 

 

N397( 41/64 DRILL TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .64063)

N398T2M6

N399G0G90S417M3E1X3.9311Y-1.7327

N400H2Z.1M8

N401G81G99X3.9311Y-1.7327Z-1.3R0-.18 F3.<--- how can i change this g99 to g98 instead i keep snaping tools off because i want to go to initial plane instead of ro plain

N402X2.6186Y-1.8401

N403X.8999Y-1.5091

N404G80

N405M5M9

N406G90H0Z0.

[3rdstring]

On the drilling parameters page Check the "Clearance" check box & set your initial plane there. Make sure the "Use clearance only at start & end of operation" is unchecked. That should give a G98 in your drill cycle.

 

HTH

[bthomps5]

tried that and it gives THE G99 INSTEAD OF G98

 

 

T3M6

G0G90S461M3E1X.8999Y-.9956

H3Z.1M8

G82G99X.8999Y-.9956Z-.9R0.1P1000F4.61

X2.6186Y-.6646

X3.9311Y-.772

G80

M5M9

G90H0Z0.

E0X0Y0

T1M6

M2

[Guest]

Can you post the pdrill$ section of your post, like the one below

 

code:

---

pdrill$          #Canned Drill Cycle

pdrlcommonb

pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout,

prdrlout, dwell$, *feed, strcantext, e$

pcom_movea

---

[bthomps5]

here we go i hope this what you are talking about

 

 

pdrill #Canned Drill Cycle - G81/G82

pdrlcommonb

pcan1, pbld, n, *sgdrill, *sgdrlref, pfxout, pfyout, pfzout, pcout,

prdrlout, dwell, *feed, strcantext, e

pcom_movea

[Guest]

Hmmm, I half expected to find a "G99" hard coded there.

 

What are your tool setting

 

Clearance

Retract

Top of Stock

Depth

 

Are they absolute or incremental

[bthomps5]

everything set to absolute

 

Clearance 0.1

Retract 0.1

Top of Stock 0.0

Depth -0.9

[Guest]

BINGO!!!!!!!!!!!!

 

Try changing your clearance to a larger number than your retract

[bthomps5]

that was the ticket now i under stand , under normal conditions it wouldnt matter but i am going back in a previous hole and using a R0- instead of r0+ anyway thank you very much that was it