Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Tef9 on March 31, 2009, 05:18:56 PM
-
Hello All,
I have played around with normal threading and I am starting to get some confidence, I am now looking at multi start threading via cnc and mach 3.
I last spoke to Hood about this here :
http://www.machsupport.com/forum/index.php/topic,10385.0.html (http://www.machsupport.com/forum/index.php/topic,10385.0.html)
My questions are as follows:
1) Do I need to have controll of the direction of the spindle?
2) Do I need a special gear train for multi start?
3) Does mach 3 multi start thread by coming in at a different angle? Will I need to vary the speed?
I am using a cnc Sherline.
The thread I would like to cut is a four way o.75pitch 9.5mm dia - straight, not on a taper...yet.
Thanks,
Andy
-
Program the thread 4 times each time start the z axis 1/4 pitch towards the tailstock. You will need and index pulse to do it.
Graham
-
That sounds simple enough, however urm....what is index-pulse? is this the way the motor works?
Thanks,
Andy
-
It is a slotted disc on the spindle that sends a pulse to Mach3 to tell it the speed and position of the spindle.
Look in ports and pins for index , and see if it is set active.
Graham
-
Ahhh I have set up an optical unit like Hood and rich with 1 slot in the disk, will that work?
Thanks,
Andy
-
Yes :)
Hood
-
ANDY,
Post a pic of the multi start thread.
BTW don't foget to make a nut also.
RICH
I only ever done one for kicks.
-
Will give it a go over the weekend and post a pic, Thanks for all the replyes so far!
Andy
Rich - I dont have an internal threading tool yet, if it arrives in time I will give a nut go as well!
-
Hi
I've done multi start threads on my mill using the same principle, just move the start up or down the Z by the required amount, only down side is that on a mill it finishes short by that amount too so you end up with each thread finishing short by the offset.
There are a few solutions that come to mind but they all involve a bit of hand coding which i try to avoid as I nearly always make a silly small mistake.
Steve
-
Surly you just change the G00 Z start value. I have not tried yet but I thought it should only be somthing like:
(1/4 z move each time based on a 1mm pitch)
G00 Z0.0000 (start 1)
G76 <thread code here>
G00 Z0.2500 (Start 2)
G76 <thread code here>
G00 Z0.5000 (Start 3)
G76 <thread code here>
G00 Z0.7500 (Start 4)
Or at lease that is what I thought, it should not affect the Z end or am I missing somthing?
Andy
-
Maybe not Andy, As I said I've never used G76 as I was using a mill to do the thread.
I literally just lowered the knee by the required amount without altering the code, quick and dirty but it got the job done.
I had to do this because I was making a small steam engine and I tapped the cast Iron valve block for the gland nut M6 fine then threaded the nut with the M6 fine die only to find the tap was M6X1.5 twin start so I had a machined casting with the wrong thread.
My solution was to make a new nut with the twin start thread to fit and it worked brilliantly, my first milled thread and a twin start to boot.
Moral of the story, don't assume the cheap tap and die set you bought 15 years ago has the right threads in it ;D M6X1.5 twin start looks very much like M6X0.75 so they must have got them mixed up in the factory!
-
Lol :), I asked an engineering company to quote me for a tap and die custom 4 start set....£600 eeek!
A while ago I cam acros an article about threading on the mill with a single toothed cutter, is somthing you have tried? I am keen to give it ago, my mill should arrive next week!
Andy
-
Yes that's what I was doing, it was actually a tool with 4 flutes and a single point in profile, if you get what I mean.
Great thing about single point is you can use the same cutter for any pitch as long as it cuts deep enough, I have a small one for around 3 -10mm and a larger one that can cut to about 4mm deep so quite large threads.
Steve
-
Bowber did you buy this tool or make it your self, ... got a pic your willing to share :o)
I was going to try making one.
Andy
-
Yes I got it from the USA via Ebay.
I'll dig out the sellers username and let you know, their not perfect but good enough to do the job.
Steve
-
That would be great.
Thanks,
Andy
-
Hm
Ebay username cmtchtools
Unfortunatly they are no longer a registered use on Ebay and the web address doesn't work either, so back to searching again, hope mine doesn't break soon.
People have used the inserts out of threading heads to make them so maybe you could search some out at Auto jumbles.
Steve
-
Hi All,
I tried to multi start thread after upgrading to the latest version, no joy yet...when displacing the start by x do you have to do the z end by the same?
i.e if I want a 1.5 pitch thread and 3 starts I displace the start point by .5 so it goes
z0 0
thread code
z0.5
thread code
z1.0
thread code
end
However in thre thread code do I need to put the thread en point .5 mm earlier?
A
-
tef9
May be wrong, but if the thread code for length was the same, then each cut would finish longer after the first thread, by the pitch / lead, because the Z start point is changing the start point. The nut would be the same thus you need not change anything on the end.
May i ask why you are doing a mut-i-start thread?
RICH
-
Have you tried the angle offset way that I pasted details about in another thread you were enquiring about multi start threads?
Hood
-
Rich - I make pens so therefore I need a smooth multi start.
Hood - no not yet, will give that a go next. The little lady has just gone back to uni so I now have some time now (i did not say that) :)
Roll on the weekend !
Andy
-
:)
Have you tried the angle offset way that I pasted details about in another thread you were enquiring about multi start threads?
Hood
Just thought I'd include the link to the "Angled Offset " approach mentioned by Hood in the earlier post.
http://www.machsupport.com/forum/index.php/topic,10385.0.html
RC
-
Good Plan,
I might try and give it a go tonight, wont be able to make a nut to test it however if it looks uniform I will count it as an improvment.
Andy
-
I have just spent 4 hours having a go at this in various ways, will post some pics and more info tommorrow night when I get back.
Andy
-
Ok...trying to be a bit more scientific about this, I have done one single start and one double start.
The single start has perfect unform looking threads, the double start seems...messy!
This method was done using the 'move the z axis' method.
any ideas as to why the second start looks messyer that the first?
I have tried the angle approach however have no pics ... yet ... will upload results soon.
Andy
-
aNDY,
So how is the angled approach working for you?
RICH
-
Hi Guys,
About a month ago I decided to try to cut a double start thread on my Emco lathe. I chucked a 15mm dia aluminum bar stock and gave it a go... and it worked perfect right on the first attempt.
I think that in order to cut multi start thread it's necessary to first understand the nomenclature and how it works. Pitch, P, is defined as the distance between two adjacent crests (for metric threads). Lead, is the distance the screw advances when it's turned one revolution. For a single start thread, lead and pitch are equal.
Thus, when you cut a (multi start) thread what you have to consider is the LEAD and NOT the PITCH. So if you want to cut a 1mm pitch double start thread, you have to program a feed of 2mm/Rev for each of the starts. Obviously, the two starts are 1mm apart, so after cutting the first lead you have to move the tool 1mm in Z and start the move from there for the second lead. Note that the depth of thread has to be the same as if you were cutting a single start thread with the same pitch (which is 1mm for this example).
Like was noted in the previous posts here, the end of cut (in Z direction) has to be adjusted for each lead so that that they end in the same point along Z.
Hope it helps ;)
BTW, Andy, both the threads on your picture above look messy. The single start thread looks awful - like mine used to be with the DC spindle motor that was not rotating steadily in the same RPM. Turned out my belt was worn out unevenly along the perimeter and was causing fluctuations in the spindle speed.
Daniel
-
Hang on I think I see you point, So if I set the pitch at 2.8mm and cut a four start thread is that an overall pitch of .7? (after increasing the z each time of course)
Andy
P.s did not think about the belt, will investigate a new one!
-
Hi Andy,
Yes. If you set the pitch in Mach3 to 2.8mm (which is actually has to be called "lead") and advance the Z axis by 0.7mm for each start, then you would get a 4 start thread with a PITCH of 0.7mm and a LEAD of 2.8mm.
Prior to getting a new belt, check how it runs on the pulley - on mine I could actually see it going up and down when looking at a fixed point just above the pulley.
Daniel
-
Thanks,
I will give it a go tonight, should have some brass rod ariving.
A
-
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
-
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
-
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?
-
This is the type of thing I use, this one if for internal.
http://cgi.ebay.co.uk/Set-of-Metric-Internal-Lathe-Threading-Tools-16mm-Shank_W0QQitemZ270292113705QQcmdZViewItemQQptZUK_Home_Garden_PowerTools_SM?hash=item270292113705&_trksid=p3286.c0.m14&_trkparms=72%3A1688|66%3A2|65%3A12|39%3A1|240%3A1318
And this is external.
http://cgi.ebay.co.uk/Index-A-Seiki-Lathe-Threading-Tool-16ER-inserts_W0QQitemZ250407563521QQcmdZViewItemQQptZLH_DefaultDomain_3?hash=item250407563521&_trksid=p3286.c0.m14&_trkparms=72%3A1688|66%3A2|65%3A12|39%3A1|240%3A1318
Graham
-
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
-
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
-
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
-
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
-
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
-
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
-
Just did two tests, first was using the degree offset #99066=0 etc
It seemed to be working when I was cutting air but when I did the actual cut it didnt shift and just tracked the previous thread. This could be a smoothstepper thing as probably it is not implemented for the SmoothStepper
Next I did the Z start position offset and it again seemed to work fine cutting air so tried it on some stock and this time it seemed to work fine. I inspected it after it was complete and it looks very good, each start seems 120 degree out and pitch seems good for the full 100mm length.
Pic below is not very good but it will let you see hopefully.
Hood
-
Hi Rich,
Don't know where you got the 0.86603 constant...? Nothing close to it in my books ;)
Yes I am cutting with a sharp V tool - don't cut large pitch threads.
Daniel
-
Hood,
Yep... this was the way it worked for me. I only tried a two start thread and it turned out perfectly!
Daniel
-
Daniel,
Check out a Machinst Handbook. Take a close look at the different forms. Peak to Peak of the sharp thread crests
are defined as H=0.86603 x Pitch for Unified Screw Threads. If you take away some of the sharp crests ( top and bottom ) then the remaining depth of the thread is defined as 0.61343 x pitch or 17H /24 where H is as stated. ;) ;)
RICH
-
Rich,
OK, thanks for the info :) Now I'll know to distinguish between the cases.
Daniel
-
Hmmm tried it again with just two starts and it did not work, I must be missing somthing somwhere, should the z axis move at the lead as mine is going really fast?
I am using the sherline (metric) profile would there be anything in there?
Andy
-
Can you do a single start thread?
With a twin start the z should move at twice the pitch, ie if you want to end up with 1mm pitch dual start then the z will move at 2mm/rev
Hood
-
Ahhh, the Z was going at about 245mm/rev hmmm could this be the problem. If so how do I get it to follow the speed set by the 'F'
A
-
Andy,
This M76 threading code is a two start thread using a Z offset for the start of the threads and keeping end of the thread passes the same. ( first pass starts at Z=0 and second pass starts at 1/2 the pitch ) but both end at the same point. Looking at the where the threading started on the end of the piece you can see they are 180 degrees out as expected. Looking where the threading finished for both passes you can see that they ended along the thread at the same point.
G00 Z0.0
G76 X0.33 Z-0.600 Q1 P0.0591 J0.004 L0 H0.005 I30 C0.01 B0.0002 T0
G00 Z.02955
G76 X0.33 Z-0.62955 Q1 P0.0591 J0.004 L0 H0.005 I30 C0.01 B0.0002 T0
Now as far as using the angle setting, you can get some intersting results but that is
a different story.
RICH
-
Andy,
Try what Hood has suggested. I am thinking it is a sync problem or not stable spindle speed.
Daniel
-
Ok will give it a go tonight and report back, I think my z axis is moving too quick!
A
-
Ahhh, the Z was going at about 245mm/rev hmmm could this be the problem. If so how do I get it to follow the speed set by the 'F'
A
That would be about correct for the example you gave, ie your revs were 120rpm and pitch was 2.1mm so that would mean 120 x 2.1 = 252mm/min
In my example above I was probably getting the terminology wrong.
Can you do a single start thread no problem?
Hood
Edit
just read again, were you meaning 245mm/rev like you said or per min?
-
Ok I will give the single start a go and post results.
A