cancel
Showing results for 
Search instead for 
Did you mean: 

Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Creator
Creator

On a HAAS UMC750  a (DWO) "Dynamic Work Offset" code G254 needs to be added after any "B" and "C" 5 axis rotary initial positioning block when machine is used as a 3+1 or 3+2 mill, then cancelled with G255 before next "B" and "C" move is positioned.

 

For (TCPC) "Tool Center Point Control" the G43 H01 code is replaced by G234 H01 for 5 axis machining and cancelled at the end with G49.

 

My question: - Can the required information be invoked/changed automatically by a conditional statement dependent on the process being used i.e. 3+1, 3+2 machining posts G254 and cancels with G255 at the end of the process, also 5 axis machining posts G234 in place of G43 and cancels with G49 at the end of process?

 

Examples (** ___ **) below show roughly what I need added or changed for both process.

 

(-------------------------------------------------------------------------------)

G254 Example: -

 

G00 G17 G20 G40 G80 G90
T1 M06
M01 ( OPERATION 1: CONTOUR )

(TOOL 1: 2" DIA SHELL MILL)
( CS#1 - XY PLANE )
S10000 M03
G90 G54 G00 B11.65 C-26.5
G254 (** Line added for 3+1, 3+2 machining **)
X-4.6 Y1.67
G43 Z3. H#3026 (G43 remains active with G254)
Z0.1 T5
G01 Z0.01 F200.
X4.6

 .....etc

....

....

G00 Z3.

G255

 

M01 ( OPERATION 2: CONTOUR )

(TOOL 1: 2" DIA SHELL MILL)
( CS#1 - XY PLANE )

G00 G90 B-35.25 C126.3

G254 (** Line added for 3+1, 3+2 machining **)

X-3.2 Y1.55

G43 Z3. H#3026

 .....etc

....

....

G255

G00 G53 Z0. M05

M01

(-------------------------------------------------------------------------------)

 

G234 Example: -

 

G00 G17 G20 G40 G80 G90
T1 M06
M01 ( OPERATION 1: CONTOUR )

(TOOL 1: 2" DIA SHELL MILL)
( CS#1 - XY PLANE )
S10000 M03
G90 G54 G00 B0. C0.
X-4.6 Y1.67
G234 Z3. H#3026 (G43 replaced by G234 for 5 axis machining)
Z0.1 T5
G01 Z0.01 F200.
X4.6

 .....etc

.....

....

G49

G00 Z3.

M01 ( OPERATION 2: CONTOUR )

(TOOL 1: 2" DIA SHELL MILL)
( CS#1 - XY PLANE )

G00 G90 B-35.25 C126.3

X-3.2 Y1.55

G234 Z3. H#3026 (G43 replaced by G234 for 5 axis machining)

 .....etc

....

....

G00 Z3.

G49 

M01

5 REPLIES

Re: Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Phenom
Phenom

I assume you are asking if a postprocessor can handle this - I would say yes. You don't say what version of NX you are working with - but depending on the version - the difficulty changes. Version 8 with postbuilder added the capability of using conditional code behind block templates - before NX/PB8 - it was easier to code TCL to jump around MOM_output_template commands. With version 10 - a new postbuilding system is introduced (Post configurator.) Also - the sample posts and OTB controls are different with each version. Maybe you are working with a CL post as well.

NX10.03
Windows 7 Pro

Re: Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Esteemed Contributor
Esteemed Contributor

What I'd do...

 

First, you need to determine the operation type for each op (planar mill / fixed axis contour/ variable axis contour/drill/etc.). This will allow you to change output depending on operation type. I use the variable mom_operation_type, and this can be done in "start of path".

 

For TCP, set the variable for G43 (mom_sys_adjust_code) to "43" or "234" (or 243?) depending on operation type

 

For DWO - I would add a word (e.g. "G_dwo") and make it modal.

Then when checking operatioin type, either enable or (VASC) disable that word ("MOM_disable_address G_dwo " or "MOM_enable_address G_dwo ")

 

In rapid move event, BEFORE the G0 motion blocks, check mom_out_angle_pos() and mom_prev_out_angle_pos() to see if anything is changing - if so, output G255.  Then have a "hardcoded" G254 block after the G0 blocks (as it is modal, it will only be output at the appropriate time).  Note you may want to "MOM_force once G_dwo" in start of path.


Now comes the hard part - dealing wil drill cycles (PTP and/or holemaking) when rotary axes change, and you do NOT have "Avoid" between the holes - you will have check if rotaries change, and if so, add a call to "MOM_rapid_move" (or otherwise handle it as you wish).  Note you may want to move to mom_cycle_rapid_to_pos, not the default mom_pos (which is at the top surface of the part)

 

Hope this helps...Ken

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


Re: Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Creator
Creator

The version I am using is NX6, for the moment I can edit the program to add the required lines, this I have done, running the program without TCPC the cutter path looks good but invoking the TCPC is giving me a tool path which starts off as expected but then creates unexpected tool path movements over a simple variable contour.

Do I have to switch a setting in NX so as the software realizes I'm using the TCPC function?

Re: Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Esteemed Contributor
Esteemed Contributor

Where are these unexpected movements seen?

- on the machine

- when you generate the op in NX?

- when you verify/simulate the operation in NX?

 

Ken

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


Re: Posting (DWO) Dynamic Work Offset and (TCPC) Tool Center Point Control

Creator
Creator

They are seen at the machine, I'm running a trial program in fresh-air but the differences can be seen between the non TCPC and invoked TCPC progam tool path.

Learn online





Solution Information