Author Topic: Climb Vs Conventional for Thread Milling  (Read 386 times)

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3896
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Climb Vs Conventional for Thread Milling
« on: March 14, 2020, 00:12:21 am »
I'd like to know the rationale for one vs the other.  It seems to me that conventional would mill slightly under size depending on deflection and backlash, and that climb might mill slightly oversize depending on details.

That being said I just conventional thread milled a 10-32 hole with a 0.120" 4 flute single form thread mill.  I programmed it as 0.190" (major diameter) and the machine screw just barely fit.  It threaded in, but required a wrench.  Just one finger on the wrench (short arm 5/32 hex key), but it needed it.  A spring pass made little difference.  I could hear it rubbing just barely, but I don't think it took off any practically measurable material.  I went back in at 0.193" and threaded in like it had been tapped with a nice fresh tap. 
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8182
    • View Profile
Re: Climb Vs Conventional for Thread Milling
« Reply #1 on: March 14, 2020, 00:51:17 am »
Bob,
Internal threading, conventional vs. climb:

My experience has been that if there is ANY wear in your Z axis, conventional milling produces oversized holes, and climb produces undersized (or right-sized) ones.

My thinking is that (with wear, again), conventional sort of 'digs in', pulling the whole tool toward the hole's wall, while climb does just what it's called -- it pushes the cutter away from the wall of the hole.

Of course, for external threading, it's just the opposite.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2275
    • View Profile
Re: Climb Vs Conventional for Thread Milling
« Reply #2 on: March 14, 2020, 13:10:40 pm »
My practical observations tell me the same. Conventional tends to 'bite in' while climb has a kind of 'skid' over the material. I work mostly with Aluminum and small diameter tools - <= 4 mm where it is quite noticeable.
Usually a climb finish pass is set by me with -0.025 mm roughing clearance which is in fact almost the mechanical precision my machine can achieve / minimal backlash of the mechanics.

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3896
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Climb Vs Conventional for Thread Milling
« Reply #3 on: March 14, 2020, 15:03:38 pm »
I guess this is kind of what I was getting at. In the past I seem to recall some of you guys making a big deal about wanting to threadmill in climb from the bottom of the hole up, and I wanted to know why.
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8182
    • View Profile
Re: Climb Vs Conventional for Thread Milling
« Reply #4 on: March 14, 2020, 15:14:00 pm »
Yeah, Bob.  I wrote a short VBS plugin to accommodate bottom-up threading.

At the time, I was making a number of "pressing molds" for fireworks comets, and they had threaded-in bronze inserts in the cavities.  I threaded the inserts on my lathe, but the 3"-4" thick 6061 Al mold plates got threaded on the mill.

For that application, climb always produced a much more accurate thread.  The nice thing about climb, too, is if you run it more than once on the same hole, it produces a more-and-more accurate profile.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3896
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Climb Vs Conventional for Thread Milling
« Reply #5 on: March 14, 2020, 16:22:37 pm »
Ok. thanks.  

FYI:  Most of you guys already know this, but on the little high speed mills (24K rpm at 39ipm programmed) Thread milling was faster than tapping similar holes on the bigger mills with more low RPM torque.  I know I can crank up the RPM and feed on the bigger mills, but for what I am comfortable with...  Its totally comparing apples to cinder blocks for a comparison, but thread milling with a high speed spindle in materials suitable for high SFPM its quite fast.  

Looking at various thread mills and their recommended pitch range for their physical diameter it might be hard to find the right thread mill for smaller coarse threads.  The thread mill I used for this has a  0.120" diameter and a recommended pitch of 32-56 TPI.  I think even the coarse (24TPI) #10 NC thread might be an issue for its tiny flutes unless you went with a very low percentage of thread engagement.  I see this as more of a problem for smaller sizes.  Maybe 1/4 inch (6.35mm) or smaller.  For larger sizes the core of the mill can still be quite strong with larger flutes.  

Funny part is I am bringing out a new product (maybe if I can get the cost and machine time down) for which I bought some 3/8-24 gun taps for fast machine tapping, and now I am considering thread milling it instead.  Those taps may go in my tap cabinet unused for a long time.

On the high speed mills I am very much hoping to eliminate tapping as a secondary operation by thread milling on the machine instead.  It will depend on tool life, but Rogue Systems has the smaller carbide thread mills pretty reasonably priced.  Sadly they don't have any larger ones so I'm stuck with more expensive ones like Melin for bigger thread milling. 
« Last Edit: March 14, 2020, 16:26:15 pm by Bob La Londe »
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline jim1108

  • Droid
  • **
  • Posts: 86
    • View Profile
Re: Climb Vs Conventional for Thread Milling
« Reply #6 on: March 14, 2020, 22:21:59 pm »
I have always had better results with climb milling for internal threads. Thread mill last longer and in the case of internal threads, you are moving up and out of the hole which is what you want so the shavings are not packed down in the hole.

We thread mill on a regular basis. Everything from 4140, 13chrome, 25chrome, Inconel, etc..

But the one thing lacking is the implementation of cutter comp in CB's thread mill plug-in.

I don't use CB's thread mill program any more because of this. I downloaded the Advent thread mill code generator and just made generic thread mill programs for the common sizes that I can import into the CB machining operation area. Its all in incremental, so just a z depth change is needed.

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3896
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Climb Vs Conventional for Thread Milling
« Reply #7 on: March 15, 2020, 19:08:08 pm »
I found this definition of cutter compensation. 

Quote
Cutter compensation or sometimes referred to as "cutter comp", is an offset or shift from center line of the tools shaft to the cutters edge along a programmed path. The advantage of cutter compensation is the use of geometry based offsets rather than tool center point, allowing for the same program to use different diameter tools.

That definition seems to mix two different things. 

That being said... if I am using two different tools I define two different tools.  I don't understand the benefit except maybe at the machine for an operator to use a different tool to do the job than somebody else programmed he job for.  However if they do that then they would also need to adjust feed and rpm for the different tool. 

For an operator who creates the code it seems to me it would be easier to just regenerate the code, or regenerate that portion of the code as a fix file than to tweak the machine. 



Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 2875
    • View Profile
Re: Climb Vs Conventional for Thread Milling
« Reply #8 on: March 15, 2020, 19:15:25 pm »
That definition seems to mix two different things.
***************
In my previous life  ;) :D ;D ;D when running Cincinnati Milltronics 10vc, cutter comp was used when undersized (regrind) endmill was used..   
My 2ยข

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540