Tapping
Hi, I need help with a Tormach Modular Tension/Compression Collet Chuck and how to program for different tap sizes within HSMworks.
Thanks!
Similar Threads:
I reluctantly purchased a tension/compression head about 4 months ago, now that's all I use.Originally Posted by rockclmbr
Unfortunately, the T/C tapping head is programmed as a regular Gcode tool.
S500M3
Approach
G1Z-???? F (10% slower than actual lead)
M4
G4P.3
G1Z.25 F (10% faster than actual lead)
M3
G4 P.3
Move to next hole repeat or paste tap cycle.
Before I got my T/C tapping head, I always used a Tapmatic head. The way I do it now is so easy, I don't use the Tapmatic any more.
You can buy GOOD PARTS or you can buy CHEAP PARTS, but you can't buy GOOD CHEAP PARTS.
Re: Tapping
Here is how I program for T/C on my 1100. Its a sub-routine I keep in the parent folder to all of my code. I set a drill operation for all the holes that need tapped just to get their location. Then when I post I open this code, copy the sub, paste in the new NC at the bottom. Copy the rest and paste above the Drill op that the post created. Copy all the drill points and paste into this code. Copy and paste the M98 P#### L1 after each drill point and delete the drill op.
Sounds like a lot but I regularly make fixtures with 100+ tapped holes and this is a hell of a lot easier than hand writing code and a lot safer for me since I'm less likely to make mistakes with copy/paste than with key strokes. Total time to program 100 holes is about 5 minutes. Total broke taps using this code to date = none. I created it when I machining pivot nuts for my production part and the first time I used it was 1,500 6-40 threads with no problems. I just ran Kool-Mist at the time then later tried the Tormach stuff and both worked fine in 7075 and 6061 (which is all I have tapped with this). Now I am using "real coolant" and freaking LOVE it: Castrol Hysol MB 50. They were supposed to bring me the 20 but brought the 50 by mistake and let me keep it anyways. Hope this helps.
Feel free to ask away if you have any questions about the routine. If you are not used to conditional programming it can be a little overwhelming.
(PASTE THIS AFTER YOUR TOOL CHANGE AND G43 H##)
( T9 | T/C TAP HEAD | H9 )
(Set Editable Parameters)
#9001=-.5 (Set Depth - MUST BE NEGATIVE NUBMER)
#9002=40 (Set Thread Pitch in Turns per Inch)
#9003=600 (Set RPM)
#9004=0.4 (Set RETRACT Height)
#9005=1 (Set RAPID Height)
(Internal Parameters)
#103=0.91 (Underfeed, 0.91 -> 9 %)
#104=[#103 * [#9003/#9002]] (feed rate adjusted for under feed)
( TAP )
T9 M6 G43 H9
G20
G0 G17 G40 G80 G90 G64
M3 S400 M8
G0 (SET FIRST POINT= G0 X## Y##)
(PASTE LIST OF DRILL PIONTS FROM DRILL OP)
M98 P1001 L1 (COPY+PASTE AFTER EACH DRILL POINT)
G53 G0 Z-2
%
(PASTE THIS AFTER THE M30)
O1001 (Subroutine to Tap)
F#104 (Set feed rate)
S#9003 (Start Spindle)
G0 Z#9004
G1 Z[#103 * #9001] (Tap down to compensated depth)
M4 (Start Spindle in Reverse)
G4 P.5 (Pause for spindle reverse)
G1 Z#9004 (Raise spindle at feed rate to rapid height)
G0 Z#9005
M3 (Start Spindle for next hole)
M99 (Subroutine Return)
%
Re: Tapping
I agree this tool get the 2 thumbs up! Worth every minute to get setup!
I use sprutcam and save default setups for tap routines that can be added to part program with a click and you have tapped holes.
Thinking most cam is the same "no experience" does take a little to setup right and test.
Anyway I need to research this again. I have it backwards from example steve shows!
I have retract feed at 90%, and approach feed at 100%
Back to the drawing board
md
Reply with Quote
