Which post processor to use for Fanuc OM controller

[Anonymous]

Please guide us. 

We are having Fanuc OM controller on 3D milling VMC. I tried Post Processor name Fanuc is not working.

Thanks 

Umesh Joshi

[GeorgeRoberts]

Hello,

Thanks for posting. What issues are you facing with the generic Fanuc post? Is there an error code / message being displayed?

Do you have some sample code that runs correctly on your machine?

Cheers

[Anonymous]

Sir,

1)I tried with Post processor 'Fanuc' it gives Alarm  Program error.

2) I tried with Post processor 'RS-274D/rs274' with this only spindle runes no axis movement.

 I have attached a sample program made on Work NC software. It works alright.

Thanks & regards

Umesh Joshi

[Anonymous]

Sir,

Sample code is attached herewith.

Regards

Umesh Joshi

[engineguy]

@Anonymous

Hi, looking at your sample code it is a little different to what is normal for Fanuc 0M, I have had several 3 axis VMC Mills over the years with Fanoc 0M control and the start of the code the Program number has always been the O and then 4 digits, like this

O1001 O and 4 numbers

Your sample code is

O01 O and two numbers

Also there is usually a % sign on the first line but your sample doesn`t have this either.

If you want the Fusion Fanuc generic post to output as per your sample then you need to modify your Fanuc Post Processor.

Before making any changes make a copy of the post and save it in a folder somewhere on your PC then you can replace it in your library if it all goes wrong

See the image below, look at Line 277 and you will see the % sign, if you delete it then it won`t be posted in the code.

Next look at Line 301, where you see the number 4 change it to a 2 and save, do not do a "save as" just click on "save".

Now try posting your code and the % should not be there and the number of digits after the O should be 2, if that is the error you are getting then hopefully that will work for you.

regards

Rob

[Anonymous]

Sir,

Thanks for the suggestion.

I tried as per your suggestion following are the results.

1)After starting the machine cycle spindle rotation started.

2)Z axis movement started upward direction(instead of downward direction) It has moved upto home position limit and stopped.

3)Spindle rotation was on .

4)I observed for few seconds and stopped the cycle.

Please suggest any other change to be done.

Regards

Umesh Joshi    

[Anonymous]

Sir,

Her I have attached the code generated after implementing your suggestion. 

Regards

Umesh Joshi

[Anonymous]

Sir,

I have some observation on difference between sample code and our generated code. Details are as follows.

1)In sample code G62 & G64 is used. In our code it is not used.

2)In sample code G54 is not used. In our code it is used.

3)In our code Z0 (Home position is called ) at the start of cycle. In sample code Z0 not called.

Does these differences cause the problem?

Regards

Umesh Joshi

[engineguy]

@Anonymous

Hi Umesh

Sorry, for the delay getting back to you, been away for a days break

Anyway, I have had a go at modifying a copy of the Fanuc Post Processor for you, looks to be fairly close to what I think you are asking for but it probably needs someone from Fusion to jump in on this one as well, I am a complete novice when it comes to modifying these Fusion Posts !!

One thing I couldn`t find a way to do was get rid of the tool length offset so I managed to get a G49 in there to cancel it in your machine control, that is something I think need the Fusion guys to script for you

Here is some code that looks close to your last sample :-

O12 (BLOCK TYPE-1)
(TOOL DIA=8. CORNER RAD=2. - BULLNOSE END MILL)
(TOOL DIA=6. CORNER RAD=1.5 - BULLNOSE END MILL)
N10 G21
N15 G00 G17 G40 G49 G80 G90 G62 G64

(2D CONTOUR-1)
(8MM R2 BULL NOSE)
N20 S8000 M03
N25 G00 X26. Y0.
N30 Z10. G49 H02
N35 G00 Z1.
N40 G01 Z-10. F333.
N45 Y21. F1920.
N50 Y26. F480.
N55 X-20. F1920.
N60 G03 X-26. Y20. J-6. F480.
N65 G01 Y-21. F1920.
N70 Y-26. F480.
N75 X21. F1920.
N80 X26. F480.
N85 Y0. F1920.
N90 G00 Z10.
N95 M05
N100 G49

(2D CONTOUR-2)
N105 M01
(6MM R1.5 BULL NOSE)
N110 S5000 M03
N115 G00 X27. Y0.
N120 Z10. G49 H03
N125 G00 Z1.
N130 G01 Z-10. F333.
N135 Y22. F1000.
N140 Y27. F250.
N145 X-20. F1000.
N150 G03 X-27. Y20. J-7.
N155 G01 Y-22.
N160 Y-27. F250.
N165 X22. F1000.
N170 X27. F250.
N175 Y0. F1000.
N180 G00 Z10.

N185 G49
N190 M30
%

The G62/G64 is the automatic corner slowdown that you can set in your control, however it can be done in Fusion under the "Passes" tab using the "Feed Optimization" option, see image below.

Also attached is a small program I did to test the code generation, run it and see if it is close to what you are doing.

Also the modified Fanuc Post for you to try out

Hope it is all of some small help to you

Regards

Rob

[Anonymous]

Sir,

Thanks for the support.

I have tried the 2d milling file and post processor you have developed. Good news is it has worked for 2D milling . Further I tried it for 3D pocket milling. Following is the observation.

1)Machine Cycle started with spindle running , X,Y,Z movement OK. 

2)The code was for cycle time 1.5 hr but after 15 min the cycle stopped. 

3) We are observing the issue to find out reason. I will be able to give further observation in next 2-3 days.

Thanks and regards

Umesh Joshi