Cancel
Showing results for 
Search instead for 
Did you mean: 

Nx Post builder help with FRN and IPM

Creator
Creator

Hi guys,

 

It's the first time I am posting on here, any help would be really appreciated!

 

I have 2 main questions for you guys:

 

 

1.  We have a 3 axis Hardinge Gx1000 with a Fanuc Oi-mc, with a Kitagawa MR200 Nc rotary table 4th axis.

 

I am currently trying to setup a post for it, I want to be able to machine 4 axis simultaneously. I know have to be in inverse time feed (FRN) and in G93 to make it work. I also need to output an F code for each line.

 

I just can't seem to figure out how to make it work in post builder? I tried importing ''pb_cmd_frn_tool_tip.tcl'' and ''pb_cmd_fix_frn.tcl'' custom commands, and I also played with Feedrate event in Program& Tool Path->Tool path->Machine control->feedrates.

 

2. Would it be possible to have 1 post for 4 axis simultaneously and 4 axis positional machining? If so, how could it be done?

 

 

Thanks!

Julien 

 

 

15 REPLIES

Re: Nx Post builder help with FRN and IPM

Phenom
Phenom

https://community.plm.automation.siemens.com/t5/Discussion-Forum-NX-Manufacturing/Rotary-FEEDs-setti...

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Nx Post builder help with FRN and IPM

Creator
Creator

Hi,

 

Thanks but i've already tried what is said in this thread... but still no luck. I can't get my post to output anything in FRN.

 

The post doesn't seem to want to output g93 or an F code at each line.

 

Here's what I done so far.

 

I also added my post, if you guys could take a look...

Any help is greatly appreciated, thanks!

 

 

 

custom commands.PNGevent_feedrate.PNG

Re: Nx Post builder help with FRN and IPM

Phenom
Phenom

hi

 

*I added some CMDs into your PP,

*also change G_feed in your motion blocks - to allow system to choose feedrate type!,

*and add "return" to your activate turbo mode command - this was problem.

   check behaviour or look inside this command and its consecvences.

*I removed you cmd from motions for forcing F.

*set back/or different feedrate modes in machine control

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #
Highlighted

Re: Nx Post builder help with FRN and IPM

Phenom
Phenom

I added force G_feed address into PB_CMD_FEEDRATE_NUMBER and PB_CMD_FEEDRATE_NUMBER_fanuc.

You can delete it if you dont want G93 on every block or

 

It is in the end of cmds:

   MOM_force once F G_feed

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Nx Post builder help with FRN and IPM

Creator
Creator

Hi Juraj,

 

Thank you very much, this solved my problem.

 

Im curious, how did you find out that the Fanuc turbo was the trouble?

 

Also, where did you find the custom CMD that you imported in my post?

 

¸Thanks again,

 

Julien

Re: Nx Post builder help with FRN and IPM

Creator
Creator

Would it also be possible to make the 4th axis lock when it's not machining simultaneously?

Can the post do this automatically? I could insert some UDE's, but I would prefer something automatic?

 

My 4 axis lock under these's M codes:

M10 = Rotary table  Brake On

M11 = Rotary table Brake Off

 

Thanks you so much for the help.

Re: Nx Post builder help with FRN and IPM

Phenom
Phenom

First, I importetd CMDs because I think they are different.

And it is maybe the same.

Maybe there are some diferences in content, but I should works and force G93 and F.

You had them already there: feedrate_number and feerate_number.

These other I had from some previous PB versions.

 

Then I realized it still doesnt work as you asked and as I expect.

So I was just trying to finding something suspicious and not familiar what I usually use in Postbuilder and try "return" from that CMD.

 

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Nx Post builder help with FRN and IPM

Phenom
Phenom

to LOCK 4th axis question:

Yes it possible.

1.

You have to decide if the tool paths of the operation are simultaneous or 3+2

(machining without rotary axis moving whether it is 4 or 5 axis machine).

 

Clue: mom_tool_path_type, mom_operation_type.

So now you handled simultaneous or 3+2.

 

2.

In the start of operation:

If tool paths is 3+2 (positioning of rotary axis and stay still)

then output your lock funtions (even for both axis).

 

In the end of operation:

If Lock funtions was outputed

then output UN-lock functions.

 

No UDE.

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Nx Post builder help with FRN and IPM

Creator
Creator

Hi,

 

Thanks it work out great with what you suggested.

 

Back to the FRN mode, I started post processing some programs. Sometimes it outputs some weird G93, even in 3 axis, for no reason.

 

Take a look at this (this is a planar milling operation) :

 

G94 G91 G28 Z0.0 M19
(**********************)
N3 (TOOL NO. 3 - EM_0.093_3F_CARB)
(**********************)
T03 M06
T06
G54 M08
G49
G05.1 Q1
M10
G00 G90 X-.1612 Y-.1596 A0.0 S10000 M03
G43 Z.4739 H03
G93 Z.3
G01 Z.2 F150.
X-.1013 F250.1123
X-.0902 Y-.159 F1358.2319
X-.0794 Y-.1568 F1357.4834
X-.0689 Y-.1532 F1357.4834

[...]
X.8269 Y-.075 F1570.785
G94 X.8275 Y-.086 F15.
X.8296 Y-.0968 F15.
X.8332 Y-.1073 F15.
X.8381 Y-.1172 F15.
X.8442 Y-.1264 F15.
X.8515 Y-.1347 F15.
X.8598 Y-.142 F15.
X.8689 Y-.1481 F15.
X.8788 Y-.153 F15.
X.8893 Y-.1565 F15.
Z.3 F15.
G93 G00 Z.4749
G94 Z.4807
X.8895 Y-.1374
Z.4858

 

 

Is there a way I can remove any G93 when i'm not using my 4th axis? In other words, I would love to be in G93 only when I use the 4th axis?

 

Thanks

 

Julien

Learn online





Solution Information