can you show us the code you are using?
I have a kitamura mycenter 3 that uses Fanus OM. When I try to do a simple ridged tap like a 1/4"x20 it does the center drill and then the drill to hole size but when the machine changes to the tapping tool the tool stats to rotate drops to the part at what ever travel height, 0.100, above part then it stops. I am told that the Kitamura machine uses a different G code for tapping than some other machines that use the same Fanuc OM code.
can you show us the code you are using?
Not sure about the 0M...
But the reference to the different G-code may mean changing the G84 to G84.1 or G84.2 (there're some others but I don't remember them offhand)
You do have an M29 S~your spindle speed on the line directly before the G84...then canceled with M28 after the G80?
As mentioned, post your code for more help.
I'll post the code tomorrow as I can't get my home laptop to load the program
Thanks for your quick response.
Here is the code Bobcad posted for Two holes tapped with a 1/4"X20 tap using the tap feature.
I cannot tell if this worked if doc. didn't come through could someone tell me how to post the*.nc file Babcad creates.
Last edited by MLDatus; 01-24-2011 at 11:39 PM. Reason: attachment
moldmkr is probably correct with the M29 S*** line being needed before your G84 line.
Also you don`t mention if this is something that worked before and not now or something new you are trying to do???
You need to have a good read of your machines Manual to see if it has been setup to do rigid tapping, a lot of older machines didn`t do it.
Your machine does have to have the correct high resolution encoder connected to the spindle (Or on the spindle motor) to be able to run rigid tapping, without it there is no feedback to the Fanuc control to synchronise the spindle speed with the Z axis feed rate. It is usually done by what is known as "swap axis" where the Spindle becomes another axis so can be under full control including synchronised to account for Z axis ball screw "backlash".
Basically if your machine is fairly old it may not have that stuff on it, I have a 1989 Bridgeport 412 VMC with the Fanuc 0M Mate (F) control and I would need to add the extra encoder and change a whole bunch of parameters to make it work. The machine has all Fanuc "Red Cap" motors including the spindle motor.
However it may be the M code may also need to be set, different MTBs often use a different M code for calling up the spindle orientation, the normal "default" on 0M is M29 but I have seen M84 used when M29 has already been used for something else like a pallet changer for example.
Go look at Parameter # 0256 in your control, if it is set to anything other than 0 then that is your M code, eg #0256 29 = M29 etc.
If it is set to #0256 0 = rigid tap not available on the machine.
Hope that`s of some help to you.
Mike....If the 0M needs to see an IPM feed rate(or needs a code for IPR), then it may not actually be stopping at the G84 but just feeding really slow.
Check also to see that the P0. is supposed to be in the G84 line.
The S2001 is too fast for a tapping operation, should be under 1000. Bobcad doesn't work well in this area, so I manually edit the tool data.
Not related to your problem, but needs fixing: The drill and tap cycles need to be cancelled with G80s
So what you're seeing in these answers is you really need to know the M/G-codes required by your machine.
Do yourself a favor and STUDY your machine manuals to learn the G-codes and their syntax.
Bobcad does not lend itself well to running a post without first tailoring it to your control. (and seems like most aren't even close)
I have started with a lot that would have caused crashes with first fixing them.
Code:N34 T04 M06 N35 S2001 M03 N36 G90 G54 X-1. Y0. N37 G43 H04 Z.1 M08 N38 G84 G98 X-1. Y0. Z-.45 R.1 P0. F.05 N39 X1. N40 M09 N41 M05 N42 G00 G91 G28 Z0. N43 G91 G28 X0. Y0. N44 T01 M06
Thank you for your response. I have a mnaual which gives a tap process but only the codes an options. Obvious the spindle rpm and Z feed have to match. But I don't think the machine is just moveing slow because the spindle stops turning also. Since the spindle only has one command S2000 M03 w/ a feed of .5 per rpm. If the spindle stops where did this command come from and if the feed is based on the spindle rpm's and there are no Rpm's how can it feed? (Just thinking out loud)
I'll look at the manual and see if I can see what a proper code should be. I have had BBC write several posts and every time they do it makes somthing else not work. Is there some one who actually knows how to write posts? My Kitamura is not a rare machine. BBC can't even write a post that puts the % sign at the beginning of the program without it makeing all my 3d programs stop working. So I have stop even asking them so far I have been able to use the cd's and my experience from other programs to find ways to make it work. I am just learning the codes that make the machine function and still have a lot to learn. So thank you for your help.