Cancel
Showing results for 
Search instead for 
Did you mean: 

Post Processor Help

Experimenter
Experimenter

I posted this in the wrong forum earlier but was directed to post here. (newbie mistake)

 

We have a very old VBM with a Fanuc Control that does not use standard drilling cycles. As a result we use a Subroutine for drilling. My post processor outputs the correct positions and the output looks as follows.....

 

N70 G00 X163.375 C1.403
N80 Z1.
N100 C11.25
N110 C22.5

 

 

I would like the post to output the following so I don't have to manually insert the M98P500 for 165 holes.

 

N6 G00 X163.375 C1.403
N8 Z1.
N10 C11.25
N12 M98P500
N14 C22.5
N16 M98P500

 

I am working with a MillTurn 3axis post and NX 11. Can anyone provide some help?

6 REPLIES 6

Re: Post Processor Help

Phenom
Phenom

Not sure if your machine supports it, (Most Fanus's do)

Consider using G66 

 

N6 G00 X163.375 C1.403
N8 Z1.

N10 G66 P500
N12 C11.25
N14 C22.5
N16 G67

Re: Post Processor Help

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

You could create A Generic Motion operation to do one hole and then instance the remaining operations.

John Joyce, Manufacturing Engineer,
Senior Aerospace

NX 11.0.2.7 Vericut 8.0.3 - Statements and opinions are mine alone and do not reflect
the opinion of my employer or any other member of the human race

Re: Post Processor Help

Phenom
Phenom
Assuming you have a postbuilder post (or will) and you wish to use a "cycle" - you could customize one of them (check box in common) and have a block template for that one that is "M98" and "P500" - two text blocks. As far as getting some motion between - you will need to add some block templates for that as well. OTB template posts usually handle axes positions in the cycle output. In NX cam - it is possible to make sure you get rapid motions between cycles (using retracts, avoids, holemaking) so the implementation in the post may not need to accomodate that. Depending on where you are at (background with PB) it may be easier just to use the generic motion option mentioned above.
NX12.02
Windows 10 Pro

Re: Post Processor Help

Gears Phenom Gears Phenom
Gears Phenom

And what if you would just put coordinates and text M98P500 into some drilling move instead of cycle block?

And you will get calling macro at every hole position.

 

G00 X163.375 C1.403
Z1

C1.403

M98P500
C11.25
M98P500

C22.5
M98P500

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

Re: Post Processor Help

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

@Juraj wrote:

And what if you would just put coordinates and text M98P500 into some drilling move instead of cycle block?

And you will get calling macro at every hole position.

 

G00 X163.375 C1.403
Z1

C1.403

M98P500
C11.25
M98P500

C22.5
M98P500


This would work as well. You could use the Legacy Drilling operation with NO CYCLE.  We do this for some probing operations.  You may need to add in the Approach Marker before the insert of the macro call.  You could then instance the operations to do the other holes.

 

It really depends on if you want to customize the post or not.

 

John Joyce, Manufacturing Engineer,
Senior Aerospace

NX 11.0.2.7 Vericut 8.0.3 - Statements and opinions are mine alone and do not reflect
the opinion of my employer or any other member of the human race

Re: Post Processor Help

Experimenter
Experimenter

Thanks for all the advice.

 

Our machine is currently broke down but I will give it a try as soon as we are running again.

Learn online





Solution Information