Is there a parameter that I can change so that I can use a feed rate without my running the spindle. When I try it now it just stops with no alarm.:confused:
Thanks
Mike
Printable View
Is there a parameter that I can change so that I can use a feed rate without my running the spindle. When I try it now it just stops with no alarm.:confused:
Thanks
Mike
You may want to program it inch per minute instead?
Ahn Vuong
I don't think there is a parameter but you might be able (but you shouldn't!!)to override it by using Keep relays.Quote:
Originally Posted by mt92
Why do you want to run the machine without the spindle running?
Maybe there's another way to do what you want to do.
Mike,
Fanuc Controlled Machining Centers control Feed in two ways, by G-Code.
1.) G94 Feed per Minute (This is usually the Default){see notes below}
or
2.) G95 Feed per Rotation (This Not Default, It is used for Tapping Primarily, and can be Used for "Controlled" Positioning {I know of a User who has a Tool Made to Pick Up a Bushing from a Gravity feed chute, and Presses it into the Just Reamed Bore!}
Fanuc Controlled Lathes control Feed in two ways, by G-Code also.
1.) G99 Feed per Rotation (This IS Default)
or
2.) G98 Feed per Minute (This is Not the Default),
G98 is Usually used on Lathe with Bar Feeder or Bar Puller because Most Lathe Logic will NOT ALLOW Axis Movement while Chuck is Open.
{see notes below}
{NOTES}
On either Machine Tool When you change (By M-code ) from the Default Feed Control Code, You must for Safety Sake Add the Default G-code after you have finished using it at the NOT DEFAULT Feed Mode back to the G-code for the Default Mode.
Be sure to be aware of this- If you are in the wrong Mode for the Feedrate, your crash will teach you to not Do that again!
A Smart Man Learns from His Mistakes....
A Wise Man Learns from Everyone's Mistakes...
JimW
I have a router mounted for engraving. and would like to run a G1 in IPM??
Mike,
Is your controller a Fanuc 6 MB?
If it is use the G-codes noted in my prior post for Machine center, not Lathe!
BTW if you have a manual and can copy / scan / e-mail the Table of contents, I'll point you to the section that covers this.
All controllers are the same in Principle, they just use different names for similar functions and some have special functions.
All should be described in your documentation. If you don't have it then that is the first thing to get!!
Then if you have questions other can help if you send the info...
JimW
I was wondering.
Is it possible to use G31.
I am pretty sure that it is in g94 as a default because that is how I always program when using the machine spindle. I cannot get it to run in a feedrate of any kind without the machine spindle running. Currently I have been using a blank toolholder and let it run 20rpm(S20M3).
Like I said. It can't be done.It's a safety thing.
I have been waiting for a chance to write this "Get a Haas".:)
I just checked: G98 G01 X-5. F5. works with the spindle stationary.
Surely there must be some way to make your machine do the same.
There may be a parameter that puts a feedhold on until the spindle is up to speed.
Normally the CNC side does not look at the spindle unless a G code for CSF or rigid tapping, feed/rev etc, and then it looks at/reads the spindle encoder.
Otherwise all M,S,T, codes are programmed through the PMC.
So it depends on the MTB as to what/how the feed rate reacts to the spindle not running when other than the above commands are issued.
Al.
Most of my W&S cnc lathes with various Fanuc controls will rapid to the feedstart position but will not start feeding until the spindle reaches the programmed speed.I`m sure the Churchills are the same.That applies to all feed commands not just canned cycles.As you say it will be a MTB decision.
Was there not a thread somewhere a while back about turning it of on a machining centre to allow flat knurling or engraving or similar?
It is possible that the control is waiting for the spindle's speed arrival in order to run the G01 after G00.
Check parameter number 6 bit 6. Example:
006 01000000 (bit 6 is active which means SAR signal is checked)
006 00000000 (bit 6 is inactive so that SAR is not checked to allow G01 command)
Give it a try.