Showing results for 
Search instead for 
Do you mean 
Reply

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

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

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

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

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

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

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