Lathe - drill feed post in FPM not IPR how can I fix this?

[Anonymous]

Im trying to drill a hole on the centerline of the part, the locations and depths are fine but when I go to post the code comes out in feet per minute not inch per rev. Im posting through the generic fanuc post for turning. This part is being turned on a fanuc OT control, is there anyway to switch this post so I can eliminate the edit?

[LibertyMachine]

Well, I spent a bit of time this morning playing around with it. My limited knowledge of post editing was not sufficient to come up with a decent solution.

I would suggest asking over here: http://forums.autodesk.com/t5/post-processors/bd-p/218

The people there are quite good about getting almost anything you need quickly. Be clear in your request and provide examples of what you are looking for and perhaps even uploading the actual post processor you are using. I'm interested to see what answer they come up with, as I am sure at some point in my future I will also have need of a good Fanuc Lathe post...

[Steinwerks]

This is definitely possible. Right now I believe the issue in the generic Fanuc post is this line:

gFeedModeModal.reset();
if (currentSection.feedMode == FEED_PER_REVOLUTION) {
writeBlock(gFeedModeModal.format((properties.type == "A") ? 99 : 95));
} else {
writeBlock(gFeedModeModal.format((properties.type == "A") ? 98 : 94));
}

Since I don't believe Drilling can bet set to FPR internally, it's pulling the feedrate from the CAM. Setting the F to the IPR value is pretty simple, but getting the G98 to G99 before the spindle speed command is trickier.

To get the F(IPR) I just changed line 862 from this:

var F = cycle.feedrate;

to this:

var F = (cycle.feedrate / tool.spindleRPM);

[HughesTooling]

Search for this line

 var F = cycle.feedrate;

Comment it out and replace with 

var F = currentSection.getParameter("operation:tool_feedPerRevolution"); 
if (unit != MM){ F = F/25.4};

Not sure why but the feed per rev was always in mm so I had to add a line to convert to inches if the document units are inches.

It should end up looking like this, it will change all the cycle feeds to per rev so be careful!!!

The feed you were getting before was spindel RPM * the feed per Rev.

Mark

[LibertyMachine]

I just tried this with a simple drill cycle on a lathe part. Works great the way you shared it Mark, Thank you!

[Steinwerks]

Both my and Mark's methods output the correct feed, but don't replace the G98 seen on line N17 here:

%
O0100 (TEST)
N10 G98 G18
N11 G20
N12 G50 S6000
N13 G28 U0.

(12 DRILL)
N14 T0101
N15 G54
N16 M8
N17 G98
N18 G97 S1000 M3
N19 G0 X0. Z1.
N20 G17
N21 G0 Z0.1
N22 Z1.
N23 Z0.1
N24 G81 X0. Z-2.2002 R0.1 F0.01
N25 G80
N26 Z1.

N27 M9
N28 G53 X0. Z0.
N29 M30
%

Hopefully he's got some more insight, because I haven't got the time to play with it although I have a few ideas. I'm still learning a lot about the post system and Mark's got me beat on that front by a very wide margin. 

[HughesTooling]

---

@Steinwerks wrote:

Both my and Mark's methods output the correct feed, but don't replace the G98 seen on line N17 here:

I was a bit worried about that as well, if it does need a G99 just try this.

    var F = currentSection.getParameter("operation:tool_feedPerRevolution"); 
	if (unit != MM){ F = F/25.4};
    writeBlock(gFeedModeModal.format((properties.type == "A") ? 99 : 95)); //Set feed per rev

This produces this code, it seems to work OK if you need to switch back to G98.

Mark

[Anonymous]

Got some time and finally was able to edit the post this works, thank you guys.

[aaronWY9GA]

I have the same situation.  I tried modifying the the default fanuc turning.cps file but am getting an error when attempting to post that states G53 is missing.  Any ideas?

[Anonymous]

I used to alter it after post and put in the codes in myself. I never
found a way around this. So from peck drilling cycles etc I had to take
what was there and modify it to fit the machine cycles later in text
format.