Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

How to change G code order?

Genius
Genius

Hello @ThomasJ

 

How to move the  D1 to the line just below the tool change? so that tool length compensation happens immediately.

 

N46 G17 X15.748 Y-7.874 A0. C0. S1400 D1 M3

 

Soft:

NX CAM 12.0.1   Post configurator

 

Controller unit:

Siemens 840D 4.5 sp2

 Machine:

DMG 160FD

5 axis millturn

Thanks

12 REPLIES

Re: How to change G code order?

Genius
Genius

and how to make the tool change to two separate line?

 

like this

 

from T1 M6

 

to T1

     M6

Re: How to change G code order?

Siemens Phenom Siemens Phenom
Siemens Phenom
Hi @SeanHAI
Are you using postbuilder or Post Configurator?
The solution is different based on the creation tool.
Regards
Paul

Re: How to change G code order?

Siemens Legend Siemens Legend
Siemens Legend

Assuming you are using post builder, edit Tool Change Auto and Manual), add th D block just under tool change block. ( I had to change the variable in D in motion as well as the new block)

ScreenHunter_03 Jun. 22 10.41.gif
%
N0010 G40 G17 G90 G70
N0020 G91 G28 Z0.0
N0030 T01 M06
N0040 D01
N0050 G00 G90 X8.7674 Y.3485 S0 M03
N0060 G43 Z.5 H01
N0070 Z-.65
N0080 G01 Z-.75 F10. M08
N0090 G41 X8.75 Y.25
N0100 Y-.25
N0110 Y-3.75
N0120 Y-4.25
N0130 G40 X8.7674 Y-4.3485
N0140 Z-.65
N0150 G00 Z.5
N0160 M02
%


ScreenHunter_02 Jun. 22 10.38.gif

Re: How to change G code order?

Gears Phenom Gears Phenom
Gears Phenom

What type of machine is this?

Typically D is the cutter compensation value and is usually on the G41/G42 line

 

John Joyce, Manufacturing Engineer,
Senior Aerospace Connecticut
www.senioraeroct.com
Production: NX11.0.2.7, Vericut 8.0.3
Development: Tcl/Tk
Testing NX12.0

Re: How to change G code order?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

@joycejo wrote:

What type of machine is this?


This syntax is used by the Sinumerik controller to indicate the tracking point, so there are many machine vendors using it.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.1, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0

Employees of the customers, together we are strong Smiley Wink
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide

Re: How to change G code order?

Genius
Genius

Siemens 840D 4.5 sp2

5 axis millturn

Re: How to change G code order?

Genius
Genius

I tried to insert a text string "\n" in *.def as shown below

Capture.JPG

 

But there is no sequence number before  M6

Capture2.JPG

Re: How to change G code order?

Genius
Genius

This is how I solved first question, I add tool_length_adjust in tool change template as shown belowCapture.JPG

Re: How to change G code order?

Siemens Legend Siemens Legend
Siemens Legend

Hello @SeanHAI,

 

you should add the D to the toolchange Blocktemplate.

toolchange_sinumerik.jpg

You should not use the \n in a Blocktemplate, it can happens that you get problems in simulation with that.

 

To get now the correct output and the seperate line just think about the MOM_suppress and MOM_force functionality. That means in the Custom procedure of the Auto Change Template you called the tool_change template 2 times, 1st with suppress M and D Address and second to force one time the D and/ or M. Thru that the post is knowing the state.

toolchange_sinumerik_2.jpg

 

 

Best regards

Thomas

 

Highlighted

How to change G code order?

Genius
Genius

Hello @ThomasJ

 

How to move the  D1 to the line just below the tool change? so that tool length compensation happens immediately.

 

N46 G17 X15.748 Y-7.874 A0. C0. S1400 D1 M3

 

Soft:

NX CAM 12.0.1   Post configurator

 

Controller unit:

Siemens 840D 4.5 sp2

 Machine:

DMG 160FD

5 axis millturn

Thanks

NX CAM Postprocessor Group
NX CAM Postprocessor Group

Members (94)