Hello Guest it is December 12, 2019, 08:24:30 AM

Author Topic: Huge Threading Problem Help  (Read 16094 times)

0 Members and 1 Guest are viewing this topic.

Huge Threading Problem Help
« on: October 22, 2010, 09:03:57 PM »
OK I think I've posted this before years ago and don't think I got a response and can't find the post.

Anyway, I'm trying to thread some 304 Stainless on my Converted 9x20 Lathe, the piece is 4 1/2" in Diameter External Threads 16 TPI at 1000 RPM with a 16 TPI Thread Insert. What happens is when it's cutting it's losing some RPMs and I know the RPM and strength of the motor is the root problem I need to solve BUT what Mach does after the second or third pass cutting is it knows the RPMs are slowing, obviously, but instead of stopping or self correcting it starts to cut at a taper and ruins the threads. Why does it do this, why would it move X inward as it's cutting. I could see it moving X for the positive to make the cut more shallow thereby making the RPM stabilize, but CUT A TAPER IN??? Please help.

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Huge Threading Problem Help
« Reply #1 on: October 22, 2010, 09:57:00 PM »
What version of Mach are you using?
I will remark that if is not 3.042.032 and above then you need to upgrade.

I would suggest you have a look at the Threading on The Lathe write-up as it will give you insight into how the threading accounts for slowing of the spindle RPM........ the range it may adjust for, what you can and cannot expect from the threading cycle. Also a whole lot of other threading related stuff.

Your threading will only be as good as your Lathe "System". I may also suggest that you just do a rough HP requirement based on the insert and
 the cut depths, the inserts, rpm, etc. I suggest you also explore using the different methods of threading. Also do some of the tests.
I don't know what type axis motors your using, in my case they are steppers, so i always have the wizard check / calculate  the number of passes which
will also display the IPM feedarate. I adjust the spindle rpm  accordingly so i am at the max power level for the steppers ( ie; below the max  axis velocity as it relates
to their torque ).
 

SS will work harder and what was easy at the first or second pass may require 2 or 3x the power to do the work hardened cut. You may be dropping below what Mach can do in recovering from a problem thread cycle ........( I have actually made the spindle briefly come to a stop and was able to recover).

BTW, on my 6" x 24" Atlas / 1/2 hp motor / 53 RPM / single 60 deg insert / modified 15 deg flank ( i think) i was able to cut a 3 1/2" x 8 x 2" long thread in steel. ( I will remark that towards the end of the threading  i thought i was going to break the carriage or tool post and made 2 or 3 spring passes)

I will say this, the threading cycle is solid if the machines system is appropriate for the task.

RICH
« Last Edit: October 22, 2010, 10:21:29 PM by RICH »
Re: Huge Threading Problem Help
« Reply #2 on: October 22, 2010, 11:04:49 PM »
Thanks. I'm using 3.042 from about a year or so ago, maybe a little newer. I switched out the motor to my old one and it seems to be working fine.

I've been cutting threads with this machine in all types of material for years and years, so I know there's nothing wrong with the machine. So my question stills stand, when the RPMs drop below what mach thinks is acceptable WHY does it start to cut a taper?

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Huge Threading Problem Help
« Reply #3 on: October 23, 2010, 11:31:30 AM »
Cartierusm,
Simple question ......maybe be a long winded reply......the answer is not simple and threading is complex.  
First just a few question's for my understanding:
-What version of 3.024.??? is it .032 or .033?
-Using exact stop and not CV?
-How much of a change in your rpm?
-Using a VFD?
-Using a single index?
-Spindle speed averaging checked / being used?
- Describe what you mean by taper.  
  Is the taper cutting over the complete threading cycle or are we talking about when the spindle slowed down?
  How much of a taper?
  What end is smaller the beginning of the thread or the end?

It is difficult to watch what is really happening when threading at say 60 ipm. I will comment that one needs to
isolate each controller reaction to a slowed down rpm in the threading cycle. There is the overall threading "picture"
and the individual parts that make up the picture. So as i continue in my reply keep that in mind as there is a lot going on.

When the rpm's drop below what mach thinks is acceptable WHY does it start to cut a taper?

Apparently a taper ( carefull as to what you mean by taper)  will be cut if say the rpm's drop, lets say 30%, and then rpm goes
back up during that cycle. As a result of the slow down, the machine must cut a varing thread pitch, not a taper over that time period.  
The "relative" thread root for that cycle would ideally remain the same since the X  axis location by code is the same / never changed
 code wise or manipulated by Mach. Because  the chip curl changed, that would create a tapered cut  and you can add cutter /  machine
 deflection to that cut taper.  Just one part of the picture.........

Mach monitors the rpm and changes the NEXT thread cycle based on how much the rpm changed. All the sampled rpm's over the cycle time
 period will provide an adjusted rpm on which to base the next feedrate. That feedrate or other feedrates over all the
thread  cycles should  provide an a properly cut thread cut. The big picture.......

Hope this simplified reply is an appropriate  answer to your question,

RICH
« Last Edit: October 23, 2010, 11:33:38 AM by RICH »
Re: Huge Threading Problem Help
« Reply #4 on: October 23, 2010, 12:03:45 PM »
Am I missing something here?  Stainless steel, 4.5" diameter, and *1000* RPM??  That is WAAAAAAAY too fast, like by 10X or more!

Regards,
Ray L.

Regards,
Ray L.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Huge Threading Problem Help
« Reply #5 on: October 23, 2010, 02:43:26 PM »
Rich is the threading expert when using the PP but I am almost certain this was an issue before Art fixed the Driver up with Rich's help, upgrade and try again would be my advice.

As for 4.5inch dia 304 threading at 1000rpm, as Ray says you are being a bit optimistic. If using carbide inserts I would be running around about the 200 to 250rpm mark.
Hood
Re: Huge Threading Problem Help
« Reply #6 on: October 23, 2010, 03:06:30 PM »
Rich, thanks for the help.
Using Version 3.042.020
Using CV
can't really tell about how much RPM loss but looks like about 30 RPM
Using VFD
Single Index
Don't know what spindle speed averaging checked is, can guess what it is but don't know where to find that option or if it should be used.

As far as the taper. Let's say I'm making .002 depth of cut per pass so it doesn't bog down the motor, I think Mach may set it's own depth of cut anyway even though this is what I have it set for in the threading wizards setting page, because it doesn't take that long to thread as it sounds with a .002" depth of cut per pass. Anyway, let's say I'm making 16 TPI threads on 4" stock. First pass will be 3.996", next pass will be 3.992, then 3.988, by this time (with the old motor) it will start to loose RPMs and instead of the next pass being at a depth of 3.984", it will start at 3.984" and go down to something like 3.9645" tapering down the run and continue if I let it. I can't really tell what the exact end depth is on X as I'm just looking at the DRO on Mach and it's moving counting down as it moves. The beginning of the thread is larger in diameter and the back end is smaller. It happens after it makes a normal pass where it starts to loose RPMs, then the next pass is tapered and it continues.

@ Himy, I can't go slower even geared down motor with a VFD if I go to 100 RPM the motor will be very weak. I assume Himy, that you have a CNC lathe that you can actually gear down to 100 RPM? I usually don't have a problem at 500-700 RPM. I was trying 1000 RPM because my motor lowered to 500 RPM was losing RPMS during threading, but last night I changed to my 2 HP motor with gearing so the highest RPM I can get is 742 rpm, so that will give me full HP at that RPM.

@ Hood, thanks also, I'll try lower speed with the motor, with the old motor back in, if it continues to work I'll put a different pulley on it to make it's top speed 350 RPM or so.
Re: Huge Threading Problem Help
« Reply #7 on: October 23, 2010, 03:18:24 PM »
@ Himy, I can't go slower even geared down motor with a VFD if I go to 100 RPM the motor will be very weak. I assume Himy, that you have a CNC lathe that you can actually gear down to 100 RPM? I usually don't have a problem at 500-700 RPM. I was trying 1000 RPM because my motor lowered to 500 RPM was losing RPMS during threading, but last night I changed to my 2 HP motor with gearing so the highest RPM I can get is 742 rpm, so that will give me full HP at that RPM.

RPM should be determined by recommended SFPM for the specific tool being used, and the material being cut, whether it's turning or milling.  Excessively high RPM will destroy the tool very quickly, and with stainless can easily lead to work-hardening, which will make the material near impossible to cut.  Most carbide tools recommend SFPM in the 1000-3000 range, but you're up at around 15,000.  You may get away with it, but it'll be really brutal on the tool.

Regards,
Ray L.
Regards,
Ray L.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Huge Threading Problem Help
« Reply #8 on: October 23, 2010, 05:23:05 PM »
I have never been keen on VFD's, they are great for varying the speed within a range but as you have found when you get down in revs they are not much use. Any commercial machines I have seen that use VFDs have much larger motors on them than would be expected for the size of the machine as that way they still have power in reserve for the lower RPMs.

My lathe originally had an 11KW induction motor and the speeds were changed in a gearbox which operated by electro magnetic clutches. It would have been a good candidate for a VFD as I could have varied within each range to give different speeds but instead I got my hands on a big AC servo which allows me to run from zero RPM up with no loss of torque.
 You probably dont have either of these options so your best bet would be to fit more pulleys for different speeds ranges, problem would be is that you would need to manually change them.

Hood
Re: Huge Threading Problem Help
« Reply #9 on: October 23, 2010, 05:39:20 PM »
@Ray, I used a different pulley and was able to thread at 200 RPM and I only lost 1 RPM, pretty good.

@Hood, what I ended up doing was ordering an actual Adjustable Motor Base which will allow me to easily change pulleys and belts without too much of a hassle. So by the time I'm dong i should be able to switch them out pretty easy without having to sacrifice when threading.

What I'm threading is some Sch.80 304 Stainless Pipe to 16 TPI. What does everyone suggest as a good cut depth for this material running at 200 RPM. I've tried .002 and .003 cut depth per pass, as you know that's total. So from 4" next cut would be 3.997" and so on. The only reason I'm asking is toward the end of the run, the last 7 or so passes it starts to get crunchy sounding and leaves little burrs. Then I have to rerun the cycle to clean it up. So I'm wondering if that's a factor of TOO little cut depth so it's scrapping instead of shearing? or too fast or little speed? Suggestions?