Printable View
Hello guys,
I have a milling machine with controller Fanuc 0i-F.
I'm trying to make a thread but when is reversing out the feed is faster and speed is same and my thread is not good.
My progrram:
M00
S100M3
G0G90G54X0.0Y0.0M8
G43Z50H4M8
S100M29
G84G98Z-42.0R2F150
Y-15.
Y-25.
Y-35.
G80
The feed is 150 and for reversing is changing to 225.
I want the feed to be same.
Any help would be really appreciated.
Check the Parameters for the machine for Rigid Tapping --thats what is causing it
Another thing to check is the m code for rigid tapping
m code a machine manufacturer dependent
M29 is a standard but i have seen a fanuc controller using m53 instead
...a work around would be to write a Macro or subprogram or what ever to G91 the Z tap depth with 1st feedrate, than 1.5xfeedrate going up. Basically a custom bore cycle.
Looks like you use feed rate per minute? Use feed per revolution. Maybe other "canned cycle" would work better.
Hi,
I assume you use FANUC because you're in the FANUC forum and you use the Metric system.
Within FANUC you can use G94 (mm/min) and G95 (mm/rev) for tapping, so two examples for a M10 x 1.5 tap:
M00
G94( MM/MIN = STANDARD )
S300 M3
G0 G90 G54 X0.0 Y0.0 M8
G43 Z50 H4 M8
S300 M29
G84 G98 Z-42.0 R2. F450. ( F=SxP 300x1.5=450 )
Y-15.
Y-25.
Y-35.
G80
M00
S300 M3
G0 G90 G54 X0.0 Y0.0 M8
G43 Z50 H4 M8
G95 ( MM/REV )
S300 M29
G84 G98 Z-42.0 R2. F1.5 ( F=PITCH )
Y-15.
Y-25.
Y-35.
G80
G94 ( BACK TO MM/MIN )
A note on feed per rev. for rigid tapping. There is a note in the Fanuc manuals that states "Even in feed per revolution mode, pulses distributed for the drilling axis are converted to a command for feed per minute. Thus, feed per rotation mode does not strictly implement feed per rotation. Accordingly, even is the spindle stops for some reason, the drilling axis does not stop."
A couple of items to check.
Is this a new issue or is this the 1st time trying rigid tapping?
If this is the 1st time trying rigid tapping. Are you sure the control is in rigid tap mode (confirmed using spindle monitor screen under system).
Check parameter;
5200.4 Override during extraction in rigid tapping.
5200.5
Hope this is of some help.
Hi oetkbyentc,
Feed/Rev. or Feed/Min is synchronized with the spindle while tapping, you can check if you want, that's why Feed Hold doesn't work during tapping, only when it's move to an other X-Y location.
Make a simple tap g-code and during tapping switch to Single Block --- change to Handle mode and use the MPG (handwheel) and turn it slowly in + or -.
You can tap with the MPG if you want, the spindle is synchronized with the Feed per Rev. probably also with Feed/Min but I didn't try that one.
It works on my FANUC (S---M29) and Mitsubishi G84 R--- Z--- F(pitch value) ,R (comma R for rigid tapping)
You can try this for normal and rigid tapping with Feed/Min and Feed/Rev.
p.s. Try this in a save and free space above your part !!!!
Not wanting to hy-jack this thread but,
We understand that Feed Per Rev is synchronized with the spindle encoder unless sudo / coderless FPR is used. So if the spindle were to stop or slow down the axis should respond in kind. But Fanucs note indicates the axis keep moving. So I would agree with what Fanuc is saying that even if you program Rigid Tap in FPR the control converts it to FPM. I would also agree with Fanucs note in that if tapping was truly IPR the threads would be perfect even if the spindle parameters were wrong and the spindle was running at an incorrect speed as the axis feed would change to follow the programmed IPR based of of actual spindle speed. But if the actual spindle speed is off the threads are off which indicates Rigid tapping runs in IPM.
Feed Hold has no bearing on the note I added. Many canned cycles / macro statements delay feed hold as you described.
Thank you for your help.
I solved by changing parameter 5200 #4 DOV from 1 to 0 and now the feed is same for both directions.
...Tapmatic vs Ridge tapping..Fanuc was thinking flexable...sweet.Quote:
Originally Posted by vanova20
Thank for the 5200 report