[easyguy97]

Hi guys...my problem..I'm running an Okuma MC600 horiz. Mill with Okuma control OSP7000M...I'm spotting,drilling and tapping alum parts, and for some reason, in just 1 spot in my program,(2 adjacent holes) the 3/4" spot drill sometimes will suddenly drill in 100% RAPID feed rate which will not slow down with neither the Rapid control knob or the feed rate control knob. It then shows an "Error 4204 Alarm D
Feed rate Command Limit Over (replacing)"
All of the other tools (drills,taps) work normally, even at the same locations...just the spot drill. I'm only feeding at 8"/min, and the parameters show max feed rate at 200"/min.
I thought it must be an error in my program causing it to rapid in drill cycle feed, but program looked ok to me...but tonight, it started doing the same thing with the next tool, a drill!
Any ideas of what might be causing this?? and why wouldn't it "stop" the machine before drilling in rapid feedrate?

ps, the rapid "pot" knob will slow the approach in rapid before reaching "R" depth, but once it starts "feeding" in rapid, the pot knob will not affect the speed..it's 100% rapid.
Thanks! Dave in St. Louis, Mo

[littlerob]

I am trying to remember (bad idea I know) but is there a decimal point behind your feedrate, IE F8. not just F8?

[easyguy97]

Yes, there is...I think my problem is a hardware problem with the machine, because the same program will sometimes run normally, and sometimes NOT...

[Superman]

Just curious, what G code are you using ?
This all sounds like a tapping cycle and/or your feeds are in G95 ( feed per rev )
Was the previous op. tapping and you didn't set it back to G94 ?
Mills run better using feed per minute (G94), but there are times when a feed per rev (G95) is easier like tapping.
---So ensure that G94 is stated at the end of each and every tool.
This stops a spotdriil from chamfering at 500mm per rev.

The "Error 4204 Alarm D Feed rate Command Limit Over (replacing)" is a feed clamp when the programmed feedrate is over a set trigger and the machine will only use the maximum rate set in the user parameters

This 'replacing' alarm also shows up when the dry-running feedrate is higher than this trigger, it really shows up in canned cycles when the option for G01 replacing G00 in canned cycles is turned ON.

[easyguy97]

Thanks superman..I'll check for g94/g95 when I go to work today...I WAS tapping previously with rigid tapping (g284 and feed "/min). I was in regular drill canned cycle g81 for the spotdrill. I'll let you know. Dave

[easyguy97]

Yep, you were right Superman! I had been rigid tapping in G95 feed mode, and somehow accidentally deleted the G94 to return to inches/min. The reason that it sometimes still ran normally, is that when I "tested" the spot drill, I hit control reset and started on that tool, which reset the G94 (machine default) and it "spotted" fine, but when I ran through the program, the previous tool (the tap) put it back in G95, and the incorrect feed rate. Thanks..I owe you! Dave

[Algirdas]

just for the future:
there is screen on OSP, showing active modal G, M codes. You can check G94, G90 presence there.