machinist@lists.ibiblio.org
Subject: Machinist
List archive
[machinist] Setting compound angle when thread cutting - Page 2
- From: Lawrence London <lfljvenaura@gmail.com>
- To: machinist@lists.ibiblio.org
- Subject: [machinist] Setting compound angle when thread cutting - Page 2
- Date: Sun, 12 Jan 2014 15:39:49 -0500
http://www.practicalmachinist.com/vb/general/setting-compound-angle-when-thread-cutting-278289/index2.html
Thread: Setting compound angle when thread cutting
-
01-11-2014, 10:54 AM #21
- Join Date
- Aug 2008
- Location
- Californeeeah
- Posts
- 1,076
-
01-11-2014, 11:00 AM #22
- Join Date
- Dec 2011
- Location
- Washington State, USA
- Posts
- 65
If you hunker down to eye level and look at a coarse thread being cut straight in, that trailing edge is a negative rake, and the leading edge a positive. The inconsistency leads to bad things, worsening with increasing pitch. We overcome that by stepping over or feeding at an angle, or both.
-
01-11-2014, 11:11 AM #23
- Join Date
- Oct 2013
- Location
- Fall River, Wisconsin United States
- Posts
- 38
-
"...I can't see the point in setting to that precision. "
Look closely at that compound dial.
Then look CLOSE at it.
No, closer!
Make a wild stab in the dark about how accurate the stamped divisions really are.
Compare them in your mind to a dividing head, a good rotary table.
Yeah, I though you'd figure it out. Not real accurate at all.
probably readable to a half division, right? You can basically split a
division with the index without too much trouble.
One div = one degree.
Split the division = 1/2 degree.
That's where it came from. -
Yes thanks, that was exactly what I was asking. I've seen some articles in magazines where the authors would sometimes get quite insistent on how one must set exactly 29.5 degrees on the compound, yet it didn't ever make any logical sense to me.
Originally Posted by maxh
From what I read, it seems the OP asked why does everyone always say exactly 29.5 and not 29.6, 29.9, 29, or 25 for example.
My guess is that since the compound is typically marked in whole degrees, 29.5 is an easy way to say "as close to 30 as reasonably easy to read by eye without going over 30.
I'd guess a reason to shoot for as close as possible to 30, rather than 25 or 20, is that it's easy to do the math for 30 to calculate how far to expect to advance the compound to reach the end point (so you can get close before starting to measure.) And the more you deviate from 30, the more the calculation will be off.
I'm assuming most already know the reasons for advancing at an angle rather than just straight in (cutting mostly on one flank rather than two so half the cutter engagement means less likely to chatter/better surface finish, cutting force pushing against direction of drivetrain so backlash kept out and cutter stays on right path, etc.)
As somebody mostly self-taught I have no "rules" I've had to follow, and I can discover whatever I feel works best for me. When I first started cutting threads I just plunged in, but I found on coarser threads I'd often get tearing on more difficult materials. Also my lathes are lightweights and coarse threads are tough on them. Changing over to infeeding with an offset compound gave much better results but setting the compound to a precise angle as I was "supposed" to was a PIA. I couldn't see any good reason it should be so, and now have my compound at roughly 25-29 degrees for a 60 degree thread, a bit less for Whitworth, and something like 40 degrees for a 45/5 buttress (obviously feeding down the 45 degree flank).
Bill I find it difficult to imagine a trained machinist of the day would have difficulty in grinding an accurate thread tool, such that they would need to modify their way of using it. If a bumbler like me can manage to grind a tool accurately, those guys should have been able to do it in their sleep! Using the V on the fish it's not at all difficult.
Nick, from what you've said, that process is how a typical thread cycle on modern CNC machines works, but I'd be keen to have that confirmed by somebody. However I'm having difficulty in imagining how that would work on a manual machine, and how you'd keep track of the figures when backing out the tool on each pass. Can you explain when comparing with how I do it?
What I do is set the compound to say 28 degrees, as above with no particular regard to accuracy, square the QCTP, touch off the tool and zero the dials. I then place a dial indicator reading off the toolpost and adjust the stand so the indicator is reading the depth of thread (I use a small Noga for that, so the depth adjustment is super easy). Make a pass, confirm the pitch, back the cross slide off, return to the start, bring the cross slide back up to zero, add a cut using the compound, engage the half-nuts and go again. If its not an especially critical thread I'll just keep doing this until my dial indicator reads zero and then I'm done. If its more critical I will begin testing the thread, either with wires or preferably with his mate, as I approach a zero reading. It's super fast, pretty much idiot proof, and its exactly the same process regardless of what type of thread I'm cutting. With the method you described, I'm puzzled as to how you keep track of the cross slide reading when you back off each time to return to the start of the thread, I just bring it back to zero each time, but won't that figure keep changing doing it your way? Also, as I said, I use exactly the same process regardless of thread form, won't your ratios change is say cutting a Whitworth, acme, or buttress thread, so how do you cut them? I'm always curious to try different ways of doing things and experiment (the latter why I initially questioned the whole insistence of this precise compound setting).
Pete -
01-11-2014, 08:52 PM #26
- Join Date
- Oct 2012
- Location
- Shawnee, Kansas
- Posts
- 12
I think it's like max said, the tool face on the leading edge does the cutting, the half degree is for relief on the trailing edge. You plunge in parallel to the trailing edge is where the 30 degrees comes from with a slight relief of 1/2 degree. It is minimal. People are specific because machinists don't do well with vague dimensions-like, set it to thirty and go back a hair wouldn't go well.
As a technique, use the compound until the last .035, take a tool pressure cut, and take three passes with the cross slide straight in. (Or something like it, just one method taught to me).
As for cnc or any machine with good rigidity, it's a straight in cut every time (I don't think the 20"x 30' LeBlond I ran had a compound) chatter is less of a factor. I had a DRO that made it easier. Speed seemed to be the key to getting a good finish-ie. as fast as you can without breaking the insert (which is a real pita to get out of half done threads). -
"the half degree is for relief on the trailing edge. "
At the risk of being cranky - No.
It is NOT relief. Relief would be where you put the compound at 31 degrees.
The 29-1/2 number is so that BOTH sides of the form tool (threading, it's a form tool
process if you think of it) take a cut. As long as both sides take a cut the thread form
is identical to the tool profile being used.
The reason that this is beneficial (compared with plunge cutting straight in) is that the
left side of the tool does most of the work.
This means one chip comes off and it has space to curl over and not interfere with a chip from
the right side.
The other reason this is beneficial is that the carriage gets loaded hard against the half nuts
in ONE direction. Improves accuracy - if the carriage is being run via ball screws in an NC
machine, not so important. But the first issue still stands even then. -
Does anyone else take "spring cuts"
If so, the path that the tool takes to get to those final passes is only to better form the chips and ease the cutting process.
During spring passes, the threading tool is a form tool.
Jeesh guys...Pay attention ;-) -
01-11-2014, 09:37 PM #29
- Join Date
- Nov 2006
- Location
- Kankakee, Illinois
- Posts
- 212
-
Originally Posted by maxh
From what I read, it seems the OP asked why does everyone always say exactly 29.5 and not 29.6, 29.9, 29, or 25 for example.That's the long way around the block for nothing. Originally Posted by Pete F
Yes thanks, that was exactly what I was asking.
Tom -
Pete F, Thermite, I'm really on your page & following your lead
, translating better into than out of my English. 
I grind to 60^ just to ease setting up with the fishtail, and set compound to ~29.5^
as an learned goldilocks increment & from success following the old
ways. I pretty much have to feed with the compound, also for having
weak TPs and to keep chatter down. btw: Bill's 'cutaway' tool example
works for me.
Having never threaded much smaller than 3/8"-16 and mostly in steel with 60^ inserts I'm going to remember all this when I jump to 1 1/2"-36 & some other oddities planned in soft metals (HSS & some 'insiders' among them), .... and I may come looking for you guys....
-
After all that noise and 26 posts, Jim is the only one who understands the reason for setting the compound that way. If you plunge, you have two equal chips trying to occupy the same space. The compound angle is not critical, just so long as it takes the main chip off one side and shaves the other side just enough to clean it up but not make a big enough chip to interfere with the main cut. Originally Posted by jim rozen
"the half degree is for relief on the trailing edge. "
At the risk of being cranky - No.
It is NOT relief. Relief would be where you put the compound at 31 degrees.
The 29-1/2 number is so that BOTH sides of the form tool (threading, it's a form tool
process if you think of it) take a cut. As long as both sides take a cut the thread form
is identical to the tool profile being used.
The reason that this is beneficial (compared with plunge cutting straight in) is that the
left side of the tool does most of the work.
This means one chip comes off and it has space to curl over and not interfere with a chip from
the right side.
The other reason this is beneficial is that the carriage gets loaded hard against the half nuts
in ONE direction. Improves accuracy - if the carriage is being run via ball screws in an NC
machine, not so important. But the first issue still stands even then.
Bill -
01-12-2014, 04:24 AM #33
- Join Date
- Jun 2006
- Location
- Munich / Germany
- Posts
- 1,514
Take a look at the picture in posting #11.Nick, from what you've said, that process is how a typical thread cycle on modern CNC machines works, but I'd be keen to have that confirmed by somebody.
There are three ways to do it. And you can select the method on a CNC-lathe by a parameter.
straight plunge, "29.5°" advance, left/right plunge.
Also, the infeed gets smaller the deeper you cut. Geometric row. Also can be defined on a CNC. First DOC say is 1 mm, second 0.5 mm, ... minimum DOC is 0.1 mm Or whatever.
It depends on the pitch. The coarser the pitch, the less the straight plunge works.
Nick -
Nick, I was mainly asking how you thread on a manual lathe. I've seen that image before, it's from a Sandvik booklet on threading IIRC
Bill, I think MOST here understand why the compound is offset v plunging. The question remains why 29 and a HALF degrees. 29 degrees will also mostly cut on one side of the tool, with the other side just enough to clean it up. Likewise 28 degrees, only very slightly less so. Likewise 27 degrees, but even less so again. The only reasonable answer I can see is that 29.5 is the closest practical value less than 30 (which would cause one side to rub.). However I can only conclude that anyone who insists this number is an absolute and "must" be set is speaking out their clacker -
01-12-2014, 10:04 AM #35
- Join Date
- May 2011
- Location
- Nova Scotia
- Posts
- 278
Not quite true. In CNC you have three choices: straight plunge, left/right plunge, or infeed on one side on whatever angle you choose. You still get to pick an angle, maybe only 29 degrees, maybe less. (Actually, on the ones I ran, we put in the included angle, so 59 deg instead of 29.5. And you can pick 29.6 - or its double - if you want.) Originally Posted by Nick Mueller
Take a look at the picture in posting #11.
There are three ways to do it. And you can select the method on a CNC-lathe by a parameter.
straight plunge, "29.5°" advance, left/right plunge.
Nick
The only difference between using 29 degrees and 29.5 is what we were taught in school way back when. Same as using 0.6495P to calculate thread depth when 0.65P works just aw well - as if the extra 0.0005 in that constant really makes a difference... but we all do it. -
When I thread on a manual lathe the compound is always set at 14.5, 30, 45, or 60. The only time I ever used the compound to infeed was for an oddball thread with an inverted angle on one side. I always felt that if the gibs were adjusted right the load from pulling the carriage was enough to keep everything in lead.
-
Probably someone wanted to use a small offset and said to put the mark half way between the graduations. Just an easy way to express a small amount. A little better than specifying a skosh. In time it became sanctified by repetition.
Reply
- [machinist] Setting compound angle when thread cutting - Page 2, Lawrence London, 01/12/2014
Archive powered by MHonArc 2.6.24.