Haas lathe tapping

[Greg_J]

Hey Guys,

My when I create a tapping program for them ST30 I get a G32 code for tapping. It G32 in and then G32 out it creates a loose thread, so I went with G84 and it works well but I can't get Mastercam to post out G84. I can some what adjust the post to change the G32 to G84 but I wasn't able to get a R value or a G80 after the cycle. I'm thinking there must be a switch that enables G84 to be used and all the proper code needed. Does anyone know how to do this?

 

The post is a MP-13 Generic fanuc 2 axis lathe post.

 

Thanks,

Greg

[K2csq7]

# Select canned cycle type, profile is direction of finish profile vector
sthdg32 : "G32"      #Cycle type G32
sthdg76 : "G76"      #Cycle type G76
sthdg92 : "G92"      #Cycle type G92
sthdg33 : "G32"      #Cycle type G32 with alternating position
sthdgcode : ""       #Target string

 

 

Find this section in your post and swap the G32's inside the quotes for G84 (keeping the quotes) so it looks like

this...

 

 

# Select canned cycle type, profile is direction of finish profile vector
sthdg32 : "G84"      #Cycle type G32             #was "G32"
sthdg76 : "G76"      #Cycle type G76
sthdg92 : "G92"      #Cycle type G92
sthdg33 : "G84"      #Cycle type G32 with alternating position                #was "G32"
sthdgcode : ""       #Target string

 

[Mr. Wizzard]

Keith has it, but double check your parameters for clearance, depth, etc...

If i remember correctly, i had to do some more monkey-ing for my Haas post to get the other parameters correct.

At least on the drilling cycles, I know i had to make more adjustments.

[Greg_J]

I was able to to do that part but it would output a "R" value and a G80 at the end of the cycle.

[Josh T™]

Greg,

 

Shoot me an email.

[K2csq7]

If this is something you will not ever need you can just take the variables out of the postblocks.

 

If you will need the functionality in the future you would be better off setting up a new postblock for a custom drill cycle.

 

By using the post debugger on my mpmaster post I see that the R value comes from here...

 

 

prdrlout        #R drill position
     if absinc$ = zero, refht_a, !refht_i           	#<<<<<<<<<<< on this line... remove the "refht_a"
     else, refht_i, !refht_a

 

 

The G80 comes from here...

 

 

pcanceldc$   	#Cancel canned drill cycle
     result = newfs (three, zinc)
     if drillref = 0, zabs = initht_a           	#Make the initht the modal Z value
     else, zabs = refht_a
     prv_zia = zabs
     !zabs
     ps_inc_calc
     prv_gcode$ = zero
     if cool_zmove = yes$ & (nextop$=1003 | (nextop$=1011 & t{:content:}lt;>abs(nexttool))), coolant$ = zero
     pcan
     if drillcyc$ <> 8, pcan1, pbld, n$, "G80", scoolant, strcantext, e$                                       	### <<<<<< just take it out of this line
     pbld, n$, sgfeed, e$
     pcan2

 

 

Removing them will cause them to never be posted.... ever....

 

If you want a simple change that you would only use from time to time... alter the postblocks to add a misc integer switch that you can set in the toolpath parameters... i.e.

 

 

pcanceldc$   	#Cancel canned drill cycle
     result = newfs (three, zinc)
     if drillref = 0, zabs = initht_a           	#Make the initht the modal Z value
     else, zabs = refht_a
     prv_zia = zabs
     !zabs
     ps_inc_calc
     prv_gcode$ = zero
     if cool_zmove = yes$ & (nextop$=1003 | (nextop$=1011 & t{:content:}lt;>abs(nexttool))), coolant$ = zero
     pcan
     if mi4$ = 1,
       [
       if drillcyc$ <> 8, pcan1, pbld, n$, scoolant, strcantext, e$
       ]
     else,
       [
       if drillcyc$ <> 8, pcan1, pbld, n$, "G80", scoolant, strcantext, e$                             	
       ]
     pbld, n$, sgfeed, e$
     pcan2