PDA

View Full Version : threading assistance



spinrow
01-10-2003, 10:19 PM
I recently turned a 1" length of brass to 7/16" and threaded it 24 tpi on a 9" SB lathe. The most difficult task was resetting the threading tool to the proper location. Additional lighting didn't help. Any help or references would be appreciated. Thanks Paul

Jim Hubbell
01-10-2003, 10:48 PM
If you mean resetting between passes, a thread dial might be needed. Tho it would seem that a 24 tpi should catch anywhere on lead-screw. But if you mean resetting after sharpening just pull chuck through by hand and adjust with cross and top slide. Top slide set at 29 deg.If I am not getting it please elaborate.

gvasale
01-10-2003, 10:58 PM
I'll figure you've go the gear train all set up to do the tpi desired. Set the compound at the 29* angle to the lethe bed. Lately I've heard the layout of the markings from some makers may be different, so use a protractor if necessary. Set the threading tool with the threading gage (some people call them "fishtails"). Your bit wants to be at 90* to the work. Move the cross slide in so that it just touches the part to be threaded and back it out a little. Move the compound in until it touches and set it to "0". Now back the cross slide out a little more so there is a small clearance. Start the lathe turning and engage the feed. Hope your turning less than 50 rpm if you're a beginner. (25 or so until you get the hang of it). BTW, check for proper markings lineup of the threading dial. Hope you have the manual on this. with the feed engaged, move the cross slide in to see the slightest scoring on the workpiece and stop. Back out 1 or 2 thousandth and set the cross slide collar to "0" Back out the cross slide. Now move the carriage back to the starting point and move the compound in 3 or 5 thousandths, move the cross slide in to the "0" and engage the feed at the right time so your chosen marks on the threading dial line up. Watch carefully as you approach the end of the cut because this is where you must quickly crank the cross slide back while disengaging the feed.
Now, move the carriage back to the starting point, reset the cross slide at "0", and move the compound in a few thoudandths and repeat. Do the same thing over and again until the depth of the threads being cut go deep enough so the top of the thread begins to take the appearance of a finished screw. If you have a proper nut, try it to check the fit. Do it without taking the part from the lathe, and you can cut more if necessary. Take your time and be careful. If you screw up the first on, don't feel bad. A lot of us did. The next one will be better.

spinrow
01-14-2003, 07:26 PM
Thanks to all--My trouble was seeing the start of the thread because of the glare from the brass and the fine thread, adding light and magnification didn't help.
What I thought I might do was put a stop on the ways to stop the carriage at the proper starting point and engage the halfnut on the same line of the thread indicator each time. Would this give automatic indexing? Thanks again. Paul

Al Messer
01-14-2003, 07:38 PM
Paul, You should be able to buy a threading indicator for your South Bend from someone on the list.

Stepside
01-14-2003, 08:56 PM
If you have a theading dial you have no problem. Just engage the 1/2 nuts at the proper number. You do not have to line anything up or even be close to the end of the thread. I like to start close to the end of the thread only to save time. If no thread dial, then do not release the 1/2 nuts but rather back the cutter out (back out at least two turns) and then run the lathe in reverse until clear of the end of thread. Then move it back in to the same number ( I always use "zero" as my number) and move the compound in the proper ammount. Repeat until threads "fit", thread wires measurement is met, or your thread mike says it is the correct size. Check in your machinist handbook for the correct OD for the thread you are cutting. For your 7/16-24UNS thread the OD is .4364 and .4292 for a class 2A thread.

[This message has been edited by Stepside (edited 01-14-2003).]

chip's
01-14-2003, 09:20 PM
spinrow,
stepside an Al make good comments. I have had to make many a thread this way, it is alot slower but it works just fine. There are several articles on making thread dials, if you want to make one. Thre are also a great many machinery dealers who could help you out.

gizmo2
01-14-2003, 09:24 PM
Here's a couple things that help me get it right. I keep a 4x jeweler's loupe and a white business card with a small magnet handy. Card magged to bottom of tool holder, shine light on it, not work, and then you can inspect the work with the loupe stuck in your eye socket. Reflected light doesn't glare so bad, and plain white background eliminates distractions.
When you are cutting at 29.5* down the flank, it is called angular depth. Double depth charts are available, and can help you calculate minor diameter. If you have the space, you can turn a short portion to minor then wait for the tool to touch. But angular depth is good to know. I keep a threading notebook, with major diameter, angular depth (how far I advanced the compound) and the class of fit I thought I got. Then when I have another job with same thread count, I have an idea how far I will need to go before I start checking fit.
One more tip and I'll stop. As you come up to full depth, the tops will go from dull to sharp. But I don't usually pick this up in time, and end up with sloppy threads. Mic the o.d. when you start, when it grows .001 you've raised a slight burr and are at full depth. That's a usable thread for most things, but too deep for others. That trick, and your notebook, will serve you well. Some day I'll learn the three wire trick and all this will be old news!

lynnl
01-15-2003, 10:19 AM
The problem with the 3 wire trick is that it takes 3 hands (at least) to do it.
If you don't have a chart of depth of threads, you can use the factor ".6495". That multiplied by the pitch (or 1/TPI) gives the single depth of thread for 75% thread engagement.

ShavingMaker
01-15-2003, 02:16 PM
OK, I admit it, I cheat. I turn the threads down near the final cuts, then shut off the lathe, grab a threading die, finish the thread by hand. I just can't get clean threads the way you're supposed to by just using the lathe.

Stepside
01-15-2003, 04:29 PM
One of the most enjoyable things to do on a lathe is cutting threads.
If you are getting really poor results there are several things to consider:
1) Material-- Wrong material=poor threads
2) Quality of set-up. are the gibs tight. Are you at the correct bit height.
3) Is the bit really sharp? I use a diamond honing stone at least and quite often 2000 grit Wet/dry paper with very light oil.
4) I also use a white chip brush and lots of cutting oil. Usually the nice dark all purpose oil.
5)Because I want them "sweet" I go about it very slowly. The speed that you do the task really affects the quality.
6) If they are quick and dirty threads for a non important job I use the cut a bit and run the die over it method. Here the quality of the die has a big effect on the quality.

spinrow
01-15-2003, 09:00 PM
Thanks to everyone for the good ideas. I am going to try them on my next threading job. Paul

snorman
01-15-2003, 10:33 PM
Turn the OD a little undersize before threading and you won't have that nasty burr at the crest to worry about. Mic a few bolts to get the idea of how much undersize you want. Tap drills are chosen to give typically 70% of thread depth so the principle is the same. Very little strength is sacrificed by doing this. Use a mating part to get a good thread fit whenever possible.

One of the chief causes of nasty threads is using 1018 CRS. This stuff is just about worthless for any type of lathe work or at least it is for me. Can't turn it, can't thread it; it breaks center drills pretty regularly. You can't even do a decent filing job on it. This stuff just wants to stick to the cutting tool and that's it.

You can get excellent results by using stress-proof steel. (1144) About the same price or cheaper I've found from the online small piece suppliers and higher tensile strength as well. You probably wouldn't want to use it for shafting unless you turn the whole length but for most everything else it's vastly superior.

Fishtails are good for getting the angles right when grinding threading tools and a thread gage(tpi) will tell you instantly if that first light pass was right. And if you need to reproduce a threaded part, the gage will ID it quickly. Every machinist should have both.

FredT
01-15-2003, 11:13 PM
I was going to just continue to lurk but can't stand it anymore. After reading all the posts about threading and double depths and single depths, I just had to join in. my method for sucess is this. Sharp tool on center, quality cutting oil. Tool ground a little pointer than the fishtail. That way it doesn't hit on the back as you are feeding to the depth of the thread. As for single and double depth, I just turn the fishtail over and most of the answers are engraved on the back. I also hate to thread 1018 as is like trying to thread three day old bubblegum.
Good Luck
Fred t

charlie coghill
01-16-2003, 12:11 AM
One thing that I have found that helps me when threading is to paint the part with layout dye. Usually blue dye works best.
Charlie