Showing results for 
Search instead for 
Do you mean 
Solved! Go to solution

Post builder questions

So I am trying to build a post proccessor for a Hurco Ultimax 1 controller and there are some small things i still need to change like the tool offset.

G00 X.75 Y-8.0104 S4329 M03
G43 Z.6 H00


In the Nx toolpath the Z offset for the tool is 0 so why is it giving me a value of .6? Is there away to cancel the tool length offset in Nx that I am not doing or does the post need to be changed?


Ive tried deleting the length compensation block, aslo tried adding in g40 after the g43 h01 block to cancel but then the g40 doesnt show up after post. 


Thanks for any input, I'll be posting more questions as I go.

question tool length.PNG





Re: Post builder questions

Z.600 is your clearance plane height either defined in your operation or your MCS clearance options.

You are getting G43 H00 which is what you are saying you want?

Not sure what your question is?


Re: Post builder questions

I don't want the G43 H00 in my program how can i remove this block in the post builder? Yes you are correct about it being the clearance plane because if i was to do a drillng operation it would not have a  Z move but instead it will have a Tool length compensation block.


G40 G17 G00 G90 G70


/( TOOLSmiley FrustratedPOT_DRILL DIAMETER:0.3750 )


T10 M06


G00 X-14.5 Y-.5 S2000 M03

G43 Z.25 H00

G81 Z-.05 R.25 F6.



Re: Post builder questions

[ Edited ]

Deleting these blocks doesnt do anything?

Accepted by topic author Button_Pusher
‎01-02-2017 01:00 PM

Re: Post builder questions

To work without G43, it should also remove blocks G_adjust and H from templates of linear and rapid moves (rapid_traverse, rapid_spindle).

Re: Post builder questions

No deleting the g code inside the tool length compenstion block does not get rid of the tool length compesation block in the program.



question length 2.PNG

Re: Post builder questions

Here is another question for you guys, if im trying to output a drilling operation M08 (flood coolant) does not appear in the code after posting but for milling operations m08 appears. In the NX toolpath for the drillin op. I made sure the coolant flood was activated in the start of path events. Where can I edit this in Post Builder?

Re: Post builder questions

Note (typically) the "M_coolant" code in the linear/rapid move event is a hardcoded "flood" coolant (NOT output by a "Coolant On" UDE).

The drill cycles don't have a hardcoded "flood" coolant word anywhere, so you could either:

- add a hardcoded M8word to the "cycle common" events

- add a "Coolant ON / Flood" UDE to the operation (or "Thru" or whatever coolant you want)


Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled

Learn online

Solution Information