Printable View
I have a Bridgeport Interact 308 w/TNC 2500. I recently lost all the parameters and had to input all the values again. Everything is back up and going except I am having problems with the Tapping Cycle. When you try and M99 the cycle you get an "Arithmatical Error" no matter what is defigned in the Cycle. Could this be related to loosing the prameters....(Battery change) or am I missing somthing else?
Hey Garageshop ,
I Do not know if you are new to this machine or not but your tapping cycle should look something like this :
TOOL CALL 6 Z S 700
L R F M06
L X+0,49 Y-0,14 R0 F MAX M13
CYCL DEF 2.0 TAPPING
CYCL DEF 2.1 SET UP-0,15
CYCL DEF 2.2 DEPTH -0,3
CYCL DEF 2.3 DWELL 0,07
CYCL DEF 2.4 F175
Z+0 R0 F MAX M99
Stop M25
I have seen your problem before but i can't remember what it was .
Good Luck
Ray
Hey RMARCH,
Thanks again for the prameter list!!!
The programs that are erroring on the tapping cycle are proven programs that have made thousands of parts. I thought the same thing when my operator told me that the tapping cycle was erroring. We wrote a simple tapping cycle by hand similar to the one you posted as well as posting one in ISO and Dialoge w/Mastercam. All the results are the same. It reads the cycle definition but give the error on the M99 line.
Thanks,
Craig
Is it possible there is a parameter related to spindle speed, inch metric values or allowable feedrates that is not set correctly?
Hey Craig , Can you Email me direct ? I want to ask you something .
[email protected]
Thanks
Ray
I have checked and rechecked the parameters. Here are the parameters and values in my machine I can find for tapping.
Minimum feed rate override (7110.0) - 100
Maximun feed rate override (7110.1) - 100
Dwell for spindle rotation change (7120.0) - 0
Advance switch point (7120.1) - 0
Spindle slow down time after reaching total hole depth (7120.2) - 0
Hey Garageshop,
The values you have are all the same as mine . The - Before the value is just a Dash and not a Minus, Right ?
Ray
yes, Just a dash.
shouldn't you have parameters for encoder counts n the spindle and control outputs and direction for the spindle?
looked up at:
http://filebase.heidenhain.de/doku/o...gb/thb2500.pdf
3410 for instance, there are many others that are somewhat related
That doesn't include the plc, hwere other things might be going on
Thanks Gus and Ray...The parameter 3410 was the problem. Actually 3410.0 was set as in the parameter list provided in the machine but in the additional prameter 3410.1 you provided in the fax that were not in the list from Bpt took care of the problem. ty ty ty!!!
Hey Garageshop, SUPER !!! Glad to hear you figured it out . I know how it is when one of your machines is not running right. I have lost many nights sleep .
Ray
Great, glad to hear it. download that tech manual I linked to, it has a lot of info not anywhere else
hi
can you help me get Heidenhain 5-axis post processor for pro/E wild fire
Thanx
Does anyone know the recommended numbers for the 3410 and 3410.1 perameters? I'm having this same exact problem, looks like they are both 0-1,999 (1.999?)
TNC2500 on interact 720 with new control
I think values of .05 will work (.05V/ms) for deceleration.
http://content.heidenhain.de/doku/om.../gb/thb360.pdf
My machine is a interact 412 with TNC2500 controller.Quote:
Originally Posted by FLjoyride
The MP 3410 = 1
MP3410.1 = 1
That's what I did, and now tapping works like a charm. The dwell time should typically be 0 right? I used 1.0 like in a program example from my manual and it worked OK until I did a deep tap and snap, there it went. Using flexible tap collets, twice the diameter is plenty deep I suppose. I was trying to go almost an inch deep with a 10-24, asking for trouble :nono:
When tapping i use a .2 dwell time and it works great.
.