Hello Guest it is October 20, 2021, 02:03:41 PM

Author Topic: Muti-start threading....  (Read 23314 times)

0 Members and 1 Guest are viewing this topic.

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Muti-start threading....
« Reply #30 on: April 20, 2009, 08:33:23 PM »
Hi All,
Been fooling with multistart threading using G76. Have no problem doing single and double start threads
but for some reason a three start thread just dosn't want to come out and haven't quite figured it out.
The third start is always about .002 to .003 inches out in lead and shows up on the third start thread.
I can see the timing is not correct since you can see it on the start of the thread.
Timing or backlash associated?   :-\
Don't know.  ???

It was interesting though!  ;)
RICH 

Offline Dan13

*
  •  1,208 1,208
    • View Profile
    • DY Engineering
Re: Muti-start threading....
« Reply #31 on: April 21, 2009, 03:00:23 AM »
Hi Rich,

Wouldn't say it's backlash, since you don't see it on single and double start threads. Why would it be there on a three start thread then?

Are you sure the math is correct?

Daniel

Offline Tef9

*
  •  89 89
    • View Profile
Re: Muti-start threading....
« Reply #32 on: April 21, 2009, 03:45:52 AM »
I had a go last night with no success as my cutter grabbed the barss rod and that 'screwed' :oD the timing.

I will try angain tonight with much more shallow cuts.

Andy
p.s I have see people using what appears to be a spike for threading (which I assume is at 60 degrees)
Is this somthing you can buy or do you have to grind your own?

Online Graham Waterworth

*
  • *
  •  2,393 2,393
  • Yorkshire Dales, England
    • View Profile
« Last Edit: April 21, 2009, 03:54:19 AM by Graham Waterworth »
Without engineers the world stops

Offline Dan13

*
  •  1,208 1,208
    • View Profile
    • DY Engineering
Re: Muti-start threading....
« Reply #34 on: April 21, 2009, 03:52:43 AM »
Andy,

I would suggest you to first make sure your spindle speed reading is rock steady. As I said, from your picture it doesn't look to be so.

Daniel

Offline Tef9

*
  •  89 89
    • View Profile
Re: Muti-start threading....
« Reply #35 on: April 21, 2009, 04:07:43 AM »
Graham - thanks - I already have somthing similar for external, however the internal threading I want to do would require a smaller diameter as some of my pens are designed around a 10mm dia cap.  Do you know of a tool that can get into smaller spaces?

Daniel - Good point and no I did notice fluctuations in speed in mach three only by one or two rpm...but when going at 120rpm that is a problem, will sort that out over the next few weeks....sadly off to london to partake in real ale drinking this weekend :o)

However my index system is a fast and loose one and needs attention.

Andy


Offline Tef9

*
  •  89 89
    • View Profile
Re: Muti-start threading....
« Reply #36 on: May 06, 2009, 06:59:07 PM »
Ok, This is drving me nuts...but  I will not be beaten.

Here is the code I use to thread.  I do everything in metric, so I opted for a 0.7mm pitch with a 2.1mm lead (three starts).

Is this code correct?

does it work for anyone else?

Help :)

Thanks

Andy

G0 G40 G18 G21 G80 G50 G90
G00 G53 X0 Z0
T101M6
G00  X0.025
G00 Z0
G00 X0
M03 S120
M08
G76 X-0.5 Z-5 Q1 P2.1 J0.006 L0 H0.25 I29 C0.025 B0.0001 T0
G00 Z0.7
G00 X0
G76 X-0.5 Z-5 Q1 P2.1 J0.006 L0 H0.25 I29 C0.025 B0.0001 T0
G00 Z1.4
G00 X0
G76 X-0.5 Z-5 Q1 P2.1 J0.006 L0 H0.25 I29 C0.025 B0.0001 T0
M9
M5
M30

Offline Dan13

*
  •  1,208 1,208
    • View Profile
    • DY Engineering
Re: Muti-start threading....
« Reply #37 on: May 07, 2009, 04:13:25 AM »
Andy,

On a lathe usually X0 is the center line of the lathe and not the part surface. From your code it looks like you X0 is the part diameter and you are cutting the thread 0.5mm deep.

0.5mm depth for a 0.7mm pitch is too deep. I use this formula to determine the depth if the thread:
[depth]=0.6134 x [pitch]

It is the exact mathematical formula. Following it you get a depth of 0.43mm (after rounding) for a pitch of 0.7mm.

Other than that your code looks OK to me.

But did you check you had a stable spindle speed and a stable speed reading in Mach? Try looking at the RPM reading in Mach without "spindle averaging" checked. How stable is it? Also look at the RPM reading while taking a cut (not threading though), does it change a lot?

Daniel

Offline Tef9

*
  •  89 89
    • View Profile
Re: Muti-start threading....
« Reply #38 on: May 07, 2009, 04:25:22 AM »
Daniel,

Thanks for that I did not think that the depth would be an issue.  I will try that tonight.

I have replaced the belt, the old one looked ok but having used it excesivly I thought a belt change would be good.

I will try later with a lesser depth.

Thanks

Andy

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Muti-start threading....
« Reply #39 on: May 07, 2009, 08:32:41 AM »
Daniel,
If you are using a sharp SHARP V tool, then DEPTH=.86603 X Pitch, assuming it's positioned
on the OD of the material. You also account for actual outside diameter and any tip radius of
the sharp v tool if setting to an outside turned diameter. There are tolerances on the major, minor and pitch diameter.  If not the, the pitch diameter may not be in tolerence post cutting.
If the threading tool is not ground to the correct angle, then thread form will not be correct.
 And good grief when you start looking at all the different standards.

The I determines how the thread will be cut, such that at 30 it would be radial infeed. As you change that
down ( i use 15 on the small lathe to get an even removal of material per pass which provides for a more consistant
spindle speed and cutting, when required) and then  you end up with a flank feed.The flank feed is based on a formula which shifts the z  based on pass depth of each individual cut to accomplish even removal of material.You can see effect by generating a G32 code.
 
RICH