random "F0."

[kkominiarek]

I've found 1 post mentioning...when using Mcam HSM.....F0. can be output by accident. (this is a logged bug)

 

I am not using HSM.......every couple of months a program will post with F0.'s in it.

 

.....very frustrating on o/n runs

 

On my op page....

feedrate, plungerate have values

retract rate always set to zero

rapid retract always checked

 

Any clue on what is causing this?

[kinglouie V]

happens to me after creating a new tool and forgetting to define on last page.

[Jimmy Wakeford from Barefoot CNC]

Could be sneaking in if in jobsetup you have calc feed from tool checked and create a new tool.

 

Could also be in post if retract feed is set to zero. There are still some situations where the post will look at the retract rate for the feed value.

Instead of changing every program you could add something like:

If feed = 0, feed = default_value

[mayday]

I have it happen also, seems to be tied to certain surfacing paths. its always at the last contour segment before the retract at the end of the toolpath. i thinks it was surf finish parallel that was doing it

[betts]

OK I'm not hijacking, but what would be the cause if you get a plunge rate and then it does not go back to feed rate on the next line, but continues at plunge rate until next "jump" with G0?

 

This happens intermittently and seemingly without cause from tool, fr, type of program,(always a sweep prg), or any other settings, and it may only happen once in a very large prg.

 

I'll have to check if the statement Jimmy used above says plunge instead of default, and then it would be close, but not the same problem.

[Jimmy Wakeford from Barefoot CNC]

In the pfr/pffr post block some posts have

 

pfr

feed

 

You can:

 

pfr

feed = fr_pos

feed

 

fr_pos contains the last positive feedrate value

[kkominiarek]

Mayday,you are correct....a finish-surface-parallel had an F0. on it's last move.

[BernieT]

Have never had this problem, but I have always either defined tools with retract rate same as feed rate or set the retract rate same as feed in tool parameters page. (Rapid Retract always checked)

[Lee.]

Never had this problem. I never rapid retract.

 

I always use my tool settings.

 

Not sure this helps tho'

[BernieT]

I think it is a mistake to put in a '0' value for retract rate. It's like asking for trouble. Put in any reasonable number, preferably the feed rate, and with rapid retract checked it shouldn't read it, but if it does for any reason, no harm done.

 

Some surface toolpaths appear to use the Plunge and Retract feedrates when making steep Z moves. Because of this, I almost always set the 3 feedrates the same when surfacing.

 

Just my $.02 .....

[Bruce Caulley]

I get this on our heidi post if the retract rate and the feed rate are set the same.

 

Bruce

[Chris Rizzo]

I encounter this situation occasionally too. When I see that alarm, I immediatly know it's caused by a under-defined tool on my part. I always set retract rate to the feed rate.

 

Think of it this way too, do you really want the tool to retract at f0. ? Probably not, if it encounters a retract move, it has to feed something.

[kkominiarek]

in a perfect world "rapid retract" would mean exactly that.....but!......i'll go with entering a retract rate however....just to be on the safe side.

 

thanks all

[Mick]

The default setup in V8 (I think) had rapid retract checked. When V9 was released, the rapid retract was unchecked. This caused me grief for a while, because I normally put in a retract feedrate of 0, and use rapid retract. Its never caused an problem with me, expect at the beginning of V9, when I missed the checking of the rapid retract, and all my retracts were F0 (machine alarms up)