User Panel
Posted: 3/12/2015 9:32:02 PM EDT
My father purchased a used lathe a year ago, and has taught himself how to use it. I'll give him credit, he went from zero knowledge to threading any barrel he can chuck.
His threads are concentric and functionally perfect, he's quite the perfectionist there, but they are rough. The threads don't look or feel smooth, you can feel the roughness when you screw on a flash hider as well. They work fine, but they are just rough. Any general ideas as to why? He's using new HSS, 60 degree cutting bit, the lathe is a South Bend, circa 1960. We've measured and found no excessive run out. |
|
Carbide does not cut as clean as a HHS cutter since a carbide insert can not be sharpened as sharp and hold that kind of edge without chipping like the carbide insert,
Guessing his passes are not shallow enough, with a couple of very shallow passes for final cuts, May be trying to thread at too high of spindle speed, Advancing on the X axis handle only (with the entire tool trying to make the entire V shape cut both sides each pass), and not the compound slide, correct angle set so it's just the tip of the tool making cuts to center and left side of the threads only (read with a advance of the angle set compound, the right hand side of the groove is cut so the insert has a right edge to glide on, with tip and left hand side of the tool is making a fresh cuts each pass; and the tool is not making a leading and trailing edge cuts all at the same time to just buck the shit out of the single cutter instead.. https://www.youtube.com/watch?v=SAO3QZHhirg |
|
A couple things -
1) Is the HSS cutter exactly at half height? Not too high or too low? 2) Cutter may be rough. Stone the edges with a medium and then fine diamond stick. I get by OK with 90 degree edges without a rake. |
|
^^^great advice, especially Dano's. Advancing the tool with the compound cuts the chip loading in half resulting in a smoother cut.
One thing I do after my last pass- I have a small stainless brush with the bristles cut down to about an 1/8" long. I spin the barrel about 300 RPM and "buff" the threads a smidge. A file card works well also. This takes a lot of roughness off of threads, even if they look smooth and clean. Chip control- is the top of the tool flat or does it have about a 5 degree rake away from your cutting face? It helps the chip curl away from the face instead of piling up. Using a dark, sulphurated cutting oil? Gibs nice and snug on the compound and carriage? I like to advance the tool only about .003 or so per pass. How much is the tool sticking out from the holder? Keep it as close as you can so the tool doesn't flex excessively. Kudos to Pop for learning a new skill! |
|
Do not plunge a 60 degree cutter at 90 degrees for thread cutting.
Angle the cutter in the compound. Make sure any gibs are tight. Even relatively worn lathes can cut clean threads if set up correctly. It just takes repeated smaller cuts. |
|
all the things mentioned above, but also make sure you have slow speed and feed and are using a decent cutting oil and (i typically thread at 50-80rpm and with a feed rate of .0064") also, he is taking a series of cuts and not hogging the entire thread out in two or three passes, right?
|
|
Pretty sure that he is just using the cross slide for his depth advance of the entire thread cut depth each pass, and why the threads are produced so rough.
So again, cross slide returns back to zero after being kicked out at the end of the pass cut and brought back in before the next cut, and the depth advance of the insert is done via the compound slide set at 29.5* to the work piece instead (insert set to 90* to the work piece in the tool holder). As for depth of each pass, all depends on the lathe, but .005 is very good for the last final two passes, and if the machine is up for it, .010" to .020" is fine after you make the initial pass to thread gauge check first to make sure that you have the machine set up correctly. Also, make sure that you are using a good threading oil, and not something like WD-40 that will break down/smoke off too fast for threading. |
|
All good advice from the previous posters.
May I suggest you buy your dad this HSS threading tool as a gift. I have one and they use disposable HSS inserts and are very well made. |
|
Excellent responses so far from folks who I can tell know how to cut threads. And congrats to your dad on picking up a new
talent! If you are wanting perfect threads, it will require going the extra mile. Perfect tool geometry will also be required. Try anywhere from 3 to 7 degrees side rake clearance angle at the most, with no more than 7 degrees under the nose. As mentioned before, cutting oil is VERY important. Different metals like different cutting oil. Try Cool Tool #2 from MscDirect for starters. Old burnt or used motor oil will also work - the thicker weight is best. Try Crisco shortening....it's a miracle cure for tapping holes. For Aluminum use kerosene or mineral spirits & HSS only. Now, I am assuming he doesn't have a Hardinge lathe & is using the leadscrew with the half-nut for engagement. If you want perfect threads, do not disengage the half-nut when you reach the end.....stop the spindle, back the cross-slide out, reverse the spindle back to a good safe engagement point, stop the spindle, move back to 0 on the cross-slide, advance the compound, turn spindle on forward & rinse & repeat. It is slower, but it will give you excellent threads. Let's assume your threadform requires you to advance the compound 0.052" from the start of the thread to the bottom of the thread. First cut 0.005", second cut is no advancement.......You want to make a dry cut second, so the tool will take what it couldn't take the first time. We call this "taking the flex out of the tool". Third cut another 0.005", flex pass of 0.0" again. Now you have removed 0.010" of the theoretical 0.052". Rinse & repeat. At 0.030" deep, back it off to 0.002" per advancement. Cut, flex pass, cut, flex pass etc etc etc. At 0.040" deep, drop the advancements to 0.001" & go to 2 flex passes in a row. At 0.048", use 3 flex passes in a row. Tool geometry is crucial...... Put a chipbreaker on the nose. If you have access to a surface grinder, grind your tool on it. It will make the tool cut like a son of a heathen motherless goat. Make sure the tool is exactly on the centerline of the spindle, or no more than 0.002" below the centerline. (Mark 1 eyeball & a loupe method) Make sure the carriage & tool post are tight. As stated before, only let the tool bit stick out as much as needed, as well as the part out of the jaws... Have fun & Good luck! :) |
|
Quoted:
The compound is there for a reason, set it to 30deg and lock the cross slide, View Quote FWIW, the generally recognized number is 29.5 degrees. You CANNOT hit the number exactly, you will always be slightly higher or slightly lower than the target value. Slightly higher than 30 and you've got problems. So most people shoot for 29.5 degrees and that gives them a small buffer zone if they over-shoot. That is enough to relieve the pressure on the non-cutting edge (it will still remove a small amount of material but will mostly just act to burnish the thread-form, yielding a smoother thread. |
|
|
Quoted:
THIS is the biggest mistake most untrained people make when threading. The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound. You can't cut with both sides of the cutter at the same time and have it turn out smooth. ETA: I can cut some pretty good threads on my old beat up A-trump http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg View Quote View All Quotes View All Quotes Quoted:
Quoted:
Do not plunge a 60 degree cutter at 90 degrees for thread cutting. Angle the cutter in the compound. Make sure any gibs are tight. Even relatively worn lathes can cut clean threads if set up correctly. It just takes repeated smaller cuts. THIS is the biggest mistake most untrained people make when threading. The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound. You can't cut with both sides of the cutter at the same time and have it turn out smooth. ETA: I can cut some pretty good threads on my old beat up A-trump http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg I am running an Atrump as well, good machine. |
|
Quoted:
I am running an Atrump as well, good machine. View Quote View All Quotes View All Quotes Quoted:
Quoted:
Quoted:
Do not plunge a 60 degree cutter at 90 degrees for thread cutting. Angle the cutter in the compound. Make sure any gibs are tight. Even relatively worn lathes can cut clean threads if set up correctly. It just takes repeated smaller cuts. THIS is the biggest mistake most untrained people make when threading. The compound is there for a reason, set it to 30deg and lock the cross slide, plunging with only the compound. You can't cut with both sides of the cutter at the same time and have it turn out smooth. ETA: I can cut some pretty good threads on my old beat up A-trump http://i241.photobucket.com/albums/ff206/devtucker/AR-45/IMG_20150127_244347_929.jpg I am running an Atrump as well, good machine. Got it for basically free, our sister plant was replacing it and they were gonna sell it for salvage. ~$150 in parts and some shimming and truing and it runs like new. |
|
I have noticed that many people run at too low of a SFM. I run 150-250SFM when threading a 1/2-28 in quality barrel steel. I back it off just a bit if running a stainless barrel.
Im using solid carbide full profile inserts, and coming back through and performing a higbee cut on the first thread to cut away the partial thread. If Im being lazy I plunge directly in X or if I have time I will alternate flank infeed. |
|
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting.
|
|
Quoted:
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting. View Quote If you set a compound at 84 degrees you can do 0.0001 feed |
|
Quoted:
If you set a compound at 84 degrees you can do 0.0001 feed View Quote View All Quotes View All Quotes Quoted:
Quoted:
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting. If you set a compound at 84 degrees you can do 0.0001 feed Just not while threading. |
|
Quoted:
Quoted:
Quoted:
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting. If you set a compound at 84 degrees you can do 0.0001 feed Just not while threading. 29.5 for threading The feed is about half the dial, so make sure you measure and watch carefully. When the off flank starts to form up you are getting close. I have been known to chase with a die for the last little bit. |
|
Was just making it clear to anyone that was listening that they weren't going to feed .0001" and get super clean threads that way
|
|
|
Quoted:
Even if you could, there's such a thing as taking too little material per pass View Quote View All Quotes View All Quotes Quoted:
Quoted:
Was just making it clear to anyone that was listening that they weren't going to feed .0001" and get super clean threads that way Even if you could, there's such a thing as taking too little material per pass it is one of those hidden tricks on a compound to get surface close enough to polish down to final size for bearings. Very shallow cuts do put a premium on tool and material rigidity. Heat buildup can be an issue with small cuts. The chip carries away significant heat. |
|
My engagement is a little wonky, so I stop, retract and reverse.
My A-trump has a good, tight foot brake that kills the motor, so I don't need a massive thread relief. |
|
Quoted:
29.5 for threading The feed is about half the dial, so make sure you measure and watch carefully. When the off flank starts to form up you are getting close. I have been known to chase with a die for the last little bit. View Quote View All Quotes View All Quotes Quoted:
Quoted:
Quoted:
Quoted:
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting. If you set a compound at 84 degrees you can do 0.0001 feed Just not while threading. 29.5 for threading The feed is about half the dial, so make sure you measure and watch carefully. When the off flank starts to form up you are getting close. I have been known to chase with a die for the last little bit. Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved. This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right. |
|
Quoted:
Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved. This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right. View Quote View All Quotes View All Quotes Quoted:
Quoted:
Quoted:
Quoted:
Quoted:
Lots of good information above! The compound probably being one of the biggest pieces that beginners don't know. It was also said to make sure your gibs are tight. If you don't know what they are a quick youtube search will show how to adjust them. They make a huge difference when threading and parting. If you set a compound at 84 degrees you can do 0.0001 feed Just not while threading. 29.5 for threading The feed is about half the dial, so make sure you measure and watch carefully. When the off flank starts to form up you are getting close. I have been known to chase with a die for the last little bit. Chasing the threads with a sharp, quality, properly adjusted die is a great way to finish them. Many machinists do not like doing this, but it is a great method. This is assuming the threads are very close to finish size before the die gets involved. This is my favorite method, by far. It takes a lot of the tedious spring and finish passes out of the equation if things are done right. Let the die do the hard work. It will also correct the pitch and thread form to a certain degree. The die will also help with the deburring process. It can help to remove the rubber cratex from the process, if done right. I tend to chase with a die when I am doing stainless...it really help to remove some of the micro galling that can form... |
|
Quoted:
That's how my buddy threads on a big lathe with transmission and brake, but on a smaller lathe without a transmission or brake there's no way I could cut power and coast to a stop in the thread relief without crashing into the shoulder. I'm using a Southbend Fourteen for reference, I don't have a problem using the halfnut and thread dial to get good threads. View Quote View All Quotes View All Quotes Quoted:
That's how my buddy threads on a big lathe with transmission and brake, but on a smaller lathe without a transmission or brake there's no way I could cut power and coast to a stop in the thread relief without crashing into the shoulder. I'm using a Southbend Fourteen for reference, I don't have a problem using the halfnut and thread dial to get good threads. I thread with NO thread relief; stopping & reversing, threading away from the shoulder is the most reliable way I've found of doing this. Doing it this way makes the thread job look factory, like it was done on a CNC lathe at the same time the barrel profile was being turned. How many factory threaded barrels have you seen with a thread relief? I have seen NONE. I'm running a SouthBend 10" and I don't have any problems "coasting" to where want. You can't cut power when you get where you want to be, you cut power before you get there. Your lathe should coast to a stop at a fairly repeatable point. I can often hit a .050" window of where I intend to be simply by cutting power.2-.3" before I want to (on a 28 tpi) stop. I then turn the chuck by hand (half-nuts still engage and dragging the carriage along) until it's at the point I want it. If you're worried about running into the shoulder and you're threading away from the shoulder then your "return" should be a on pass where you aren't cutting; retract the cross-slide all the way back so even if you overshoot the shoulder it won't crash. I just did a barrel shorten/thread job for a guy. This is what he emailed me this morning, From Customer on another forum:
I can't tell you how pleased I am with the work you did on my upper and barrel. The rifle is finally starting to take shape, and now I need to start thinking about the insides of this thing so I can actually shoot it. I found an article on one of the forums about cutting a BCG for a Glock magazine. Let me know if this is something you'd be interested in working on. http://www.ar15.com/archive/topic.html?b=3&f=15&t=604491 Customer satisfaction is a testament: the entire time he was there picking up his upper/barrel he kept commenting at how professional and "factory like" the thread job looked. To each his own, whatever you prefer will most likely function the same no matter what. Just trying to point out that there are ways to skin the cat that you may have not thought of. |
|
I'm just a noob with a 7x14 mini lathe, but I'm able to cut decent threads if I do the following:
1) stiffest HSS cutter I can fit. 2) Gibbs tight. Otherwise tool will chatter and give rough threads 3) Tool on-center or a hair below center. Above-center it will dig-in as it flexes (I actually part upside-down/reverse because of tool/post flex) 4) 29.5 degree compound. Straight-in is no bueno. 5) Keep the half nut engaged the entire time. Back out and reverse with each pass. I took my threading dial off and thew it in a junk box. This method is slow but is most accurate 6) Check half-nut engagement constantly Failure of any item #1-4 would give me rough surface. If I don't do #5-6 and instead disengage the feed and use the threading dial I get very inconsistent passes. I can almost always trace rough surface finish to flex of some sort: Tool flex, Tool-post flex, loose gibbs flex, unsupported work flex, etc. |
|
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light:
That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the zero mark on the compound angle, at the *wrong* place! And they never put this 'minor' fact in their manuals, and nobody ever talks about it. You need to put the compound at 30 degrees. So you put the mark on the 60 number!! Just plain nuts. View Quote Since I've made this change my threads are perfect and super clean. |
|
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light: Since I've made this change my threads are perfect and super clean. View Quote View All Quotes View All Quotes Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light: That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the zero mark on the compound angle, at the *wrong* place! And they never put this 'minor' fact in their manuals, and nobody ever talks about it. You need to put the compound at 30 degrees. So you put the mark on the 60 number!! Just plain nuts. Since I've made this change my threads are perfect and super clean. I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a scale that reads backwards. |
|
Quoted:
I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage. View Quote View All Quotes View All Quotes Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light: That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the zero mark on the compound angle, at the *wrong* place! And they never put this 'minor' fact in their manuals, and nobody ever talks about it. You need to put the compound at 30 degrees. So you put the mark on the 60 number!! Just plain nuts. Since I've made this change my threads are perfect and super clean. I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage. I think that he thinks that the scale is double-angle, not reverse angle (90deg off) |
|
Quoted:
First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are. http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg View Quote View All Quotes View All Quotes Quoted:
Quoted:
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light: That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the zero mark on the compound angle, at the *wrong* place! And they never put this 'minor' fact in their manuals, and nobody ever talks about it. You need to put the compound at 30 degrees. So you put the mark on the 60 number!! Just plain nuts. Since I've made this change my threads are perfect and super clean. I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage. I think that he thinks that the scale is double-angle, not reverse angle (90deg off) First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are. http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg when I thread with the exception of plastic... I never take a larger than .004" depth of cut and finish with .001" and "Clear" passes |
|
|
Quoted:
First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are. http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg View Quote View All Quotes View All Quotes Quoted:
Quoted:
Quoted:
Quoted:
Here's something I just ran into using my South Bend. If you put the compound at 29.5* using the scale on the compound, you won't actually be at 29.5*. Set the compound at 59.5* to get the desired 29.5* setting. I too was having crazy rough threads using the same techniques that gave me perfect threads on other lathes. Turns out South Bend and Hardinge are both like this, in that if you're cutting a 60* thread you put the pointer at the degree of thread you're cutting instead of halfing it. Here's a quote from Practical Machinist that made me see the light: That's OK, this is the single biggest error that novices make, and it is ENTIRELY
understandable because the SB folks, in their infinite "wisdom" put the zero mark on the compound angle, at the *wrong* place! And they never put this 'minor' fact in their manuals, and nobody ever talks about it. You need to put the compound at 30 degrees. So you put the mark on the 60 number!! Just plain nuts. Since I've made this change my threads are perfect and super clean. I'll have to go home and see what you're talking about but are you sure your post shouldn't say 60.5*?? 59.5* would correspond to 30.5* on a backwards reading gage. I think that he thinks that the scale is double-angle, not reverse angle (90deg off) First, I'm not an expert on this lathe at all, so take that into account. I just followed the advice from that thread on Practical Machinist and my threads went from the example on the bottom to the example on the top just by making that one change. I know I could even make the top look nicer if I used a good aluminum cutting fluid and took smaller cuts instead of the 0.10 cuts I was taking. I'll give setting the compound at 60.5* a try and see what the results are. http://i4.photobucket.com/albums/y143/AEnemaBay/20150528_124712_zpspdr0qxbl.jpg Take a thread pitch gage and put against those threads. You might be using a 60deg cutter, but those aren't 60deg threads, they look closer to 80deg. |
|
Quoted:
Take a thread pitch gage and put against those threads. You might be using a 60deg cutter, but those aren't 60deg threads, they look closer to 80deg. http://www.roymech.co.uk/images/Iso_thread.gif View Quote I couldn't get it to focus using my phone but the pitch gauge fits well. I did get a little aggressive filing the tops of the thread: |
|
You can also trig it out with an indicator.
Multiply 29.5 tan x 1.000". The result is the length of the Opposite (short) leg of the triangle. If you travel exactly 1.000" with the cross-slide, that result should be what you shoot for. In other words, zero your Z axis & move it in X axis 1.000" & touch the same point on the indicator. When the Z axis travel amount is the same as the result you are good to go. You do not have to be exactly on 29.5 degrees. CNC lathes can cut at 90 degrees & have flawless threads. Manual machines are less rigid & it works better for them if they feed in on an angle. |
|
Other sources of rough threads -
- vibration from the motor or even slightly out of adjustment headstock bearings, - unbalanced drive belts; if your lathe uses matched belts, but they don't, take one off it's probably not needed for gun work, - wimpy tool holders or loose cutting tools (that one might have been covered already), - an out of balance chuck, - a single phase motor. Sometimes mounting the motor off the lathe helps, but the belt(s) can't flop around. |
|
Sign up for the ARFCOM weekly newsletter and be entered to win a free ARFCOM membership. One new winner* is announced every week!
You will receive an email every Friday morning featuring the latest chatter from the hottest topics, breaking news surrounding legislation, as well as exclusive deals only available to ARFCOM email subscribers.
AR15.COM is the world's largest firearm community and is a gathering place for firearm enthusiasts of all types.
From hunters and military members, to competition shooters and general firearm enthusiasts, we welcome anyone who values and respects the way of the firearm.
Subscribe to our monthly Newsletter to receive firearm news, product discounts from your favorite Industry Partners, and more.
Copyright © 1996-2024 AR15.COM LLC. All Rights Reserved.
Any use of this content without express written consent is prohibited.
AR15.Com reserves the right to overwrite or replace any affiliate, commercial, or monetizable links, posted by users, with our own.