Shop Doc Forum » CNC Swiss

1. Anonymous
   Unregistered

   We can’t accurately control the depth of the tap on our CNC Swiss lathe. The type of component we are making has a blind hole that goes .200” deep. The threads are 6 -32 and need to have a fully formed thread of a minimum depth of .185”. The tool is a thread forming tap with a blunt point. We are using a Floating Tap Collet, and we program about 10% slower than the tap pitch, stop the spindle, slight dwell, then feed off at 100% of the tap pitch. We’ve tried many variations of this method with different spindle speeds, different floating collets and different tool positions, however, we still cannot accurately control the depth. One of the issues of not being able to control the depth is that we “bottom out” frequently and break the tap. Down time, tool cost and scrap material is eating into our profit margin for this job.

   Posted 2 years ago #

2. Anonymous
   Unregistered

   One option would be to use rigid tapping if the machine has that option. Depths should repeat within .005" with this method. A second option would be to thread mill it. There are small thread mills commonly available now. Cycle time and accuracy should be as good or better.

   John Corrigan
   Technical Sales Specialist
   Technical Equipment

   Posted 2 years ago #

3. Anonymous
   Unregistered

   I have dealt with that problem, and the main problem has been chip clearance. If you have spiral taps where the chips actually peel out of the hole that's great, but I have found that to not always work. My best result has been with 2 taps with a chip cleaning effort in between.
   If you can only use one tap, then go in to .150, clean and finish.
   I made a floating tapping device that had simple cams for entry and retract that would feed to a depth stop, continue for the cam length (a 1/16" roll pin) then release at which time a reverse of the spindle would retract the tap. The failure mode is usually the roll pin breaking, leaving the tap intact and easily removed.
   I know you can buy those things, but they seem to have rubber stops or something.
   I'd be happy to send you my design.
   Tom

   Posted 2 years ago #

4. Anonymous
   Unregistered

   I agree with Tom, I avoid floating tap collets as much as possible, and rigid tap every hole I can. We have also gotten away from cut taps, and gone with all form taps when the material allows. Asking for better than +/- .005 on a thread that is tapped is a pipe dream. If you need a better tolerance, you will have to single point, IMO.

   Posted 2 years ago #

5. Anonymous
   Unregistered

   Try using an Emuge brand roll tap in a rigid holder. These are high performance taps and cost a bit more but are well worth the investment. Your current taps may not be giving you enough cutting oil removal causing a hydraulic effect during this operation. These taps are more fluted which allows for better cutting fluid evacuation. Feed at 80% pitch in and 100% out. Stay away from the floating holders.

   Posted 2 years ago #

RSS feed for this topic

Reply

You must log in to post.