Tapping threads on VM1- from MasterCam

[mafitch7479]

Can anyone give me a general idea on what the process for tapping holes on a VM1 would be? We program everything we do in MasterCam, and we've got a product we're trying to get started that has four 3-48 cap screws that are 0.25" long. So we've got 0.075" of clearance, plus 0.25" of scrap that gets removed later, and then the threads would need to be at least 0.175" (0.2" would be better).

We've never done any tapping on the mill, it's always been by hand, so I'd like a general idea of how it's done, if there's any special tooling or coding or anything that I need to know about, or how the heck to program it in MasterCam

Thanks in advance!

[mfgbydesign]

Thread Milling. Works great for large shallow threads. Tooling would be cheaper, HP requirements a lot less, size and depth control outstanding.
You can single point with a boring bar to prove the concept then buy a thread mill when you want to speed things up.
Start at the bottom of the hole and helical interpolate out. Haven't done it with Mastercam, but in Surfcam it's a breeze, can't be much different.

[mafitch7479]

Thread Milling. Works great for large shallow threads. Tooling would be cheaper, HP requirements a lot less, size and depth control outstanding.
You can single point with a boring bar to prove the concept then buy a thread mill when you want to speed things up.
Start at the bottom of the hole and helical interpolate out. Haven't done it with Mastercam, but in Surfcam it's a breeze, can't be much different.

What about small threads? We're talking 3-48 and smaller here.

[mfgbydesign]

Sorry, I misinterpreted your post as 3-inch not #3.
Mastercam (not right in front of me) has an excellent module for tapping and if the post is set up properly should be seamless.
I use a 90 degree countersink to spot the hole to the major diameter.
Tap drill size according to a chart that gives you 65% or better thread engagement. Give yourself 1/4" or better depth on the drill than you want threads if possible.
Use conservative speeds on the tap, especially with a blind hole since the Z axis will keep moving after depth is reached until the spindle stops and reverses.
Use a collet if your machine has rigid tapping otherwise you will need a floating tap holder.
The specific tap depends on the material and whether the holes go thru or not. Gun taps are the strongest but push chips ahead. Spiral flute taps pull chips. Bottom taps for shallow holes have only 3 threads chamfer (not good for hard material). H limits depend on thread tolerance (2B or 3B) generally a GH3 maybe a H5 for looser tolerance. Get go-nogo thread plug gages to check threads (not a bolt). Turn the Go gage in all the way and count turns until it comes out to determine depth.

[Brock_r]

Great sound advise from mfgbydesign.

Refer to the attachment for a Hurco NC Tap, both standard tap and rigid tap from the nc manual.

[mfgbydesign]

When I wrote "floating" holder what I meant was "tension / compression" holder.
For the tap use a 0.250 clearance plane. That gives the spindle & lead screw a bit more time to settle into synchonization before cutting.

[jetski]

I don't know how difficult of parts you are programming so this comment may not be of any use. I do injection mold tools and use the conversational side of the Hurco, and Ridged tap option and have great results. Due to the parts we mold I am able to do 85-95% of my programming with the conversational. As far as MasterCam I have version 8 and have never used it to tap. If you have the ISNC option I think you would be able to peck tap if you have the ridged tap option. Ask Hurco for sure on this Applications Engineering.