Home |
Search |
Today's Posts |
|
Metalworking (rec.crafts.metalworking) Discuss various aspects of working with metal, such as machining, welding, metal joining, screwing, casting, hardening/tempering, blacksmithing/forging, spinning and hammer work, sheet metal work. |
Reply |
|
LinkBack | Thread Tools | Display Modes |
|
#1
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNCmill with LinuxCNC
My guy asked me to cut a 1mm pitch thread on a custom shaft.
I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i |
#2
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On 2013-03-22, Ignoramus3931 wrote:
My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i And here's the subroutine, released under GPL v3 (Makes a thread on a round part rotated in my fourth axis) (Uses a 60 degree end mill) Othread_on_fourth_axis sub #x0 = #1 (X0, left side) #x1 = #2 (X1, right side) #y = #3 (Y, middle of the top edge of the round) #z0 = #4 (Z, top of the edge of the round) #safez = #5 (Safe Z for rapids) #zstep = #6 (Z Step, positive) #spr = #7 (Step Per Revolution, Also determines Total Depth) #depth = #8 (Depth of thread, positive, determined automatically if 0 based on 60 degree thread.) #diameter = #9 (Diameter of the round, needed for calculations of feed rate) #frate = #10 (feed rate based on surface speed) #left_handed = #11 (Set to 1 if left handed) #rpm = [#frate/3.1415/#diameter] #horizontal_feedrate = [#rpm*#spr] #vertical_feedrate = [#frate/5] #total_angle = [ 360 * [#x1-#x0]/#spr ] (Set negative total angle if left handed thread) Oif if [#left_handed NE 0] #total_angle = [-#total_angle] Oif endif Oif if [#depth EQ 0] ;#depth = [#spr*1.73205/2] (depth = spr * sqrt 3 / 2 ) ; http://upload.wikimedia.org/wikipedi...-p21--v001.png #depth = [#spr*0.64952] (depth = spr * sqrt 3 / 2 ) Oif endif Owithdraw call [#safez] G0 A0 (go to 0 degree) G0 X[#x0] Y[#y] Z[#safez] ( Start drilling down to Z0, I could rapid, ) ( but slow is safer, will not break end mill ) G1 Z[#z0] F[#vertical_feedrate] #direction = 1 (1 is right, 2 is left) #z = #z0 Oloop while [ 1 ] #z = [#z - #zstep] Oif if [#z LT [#z0 - #depth] ] #z = [#z0 - #depth] Oif endif G1 Z[#z] F[#vertical_feedrate] (Depending on direction, we go to X1 on the right and turn total_angle,) (or go to X0 on the left and go back to ZERO angle) Oif if [#direction EQ 1 ] #direction = 0 G1 X[#x1] A[#total_angle] F[#horizontal_feedrate] Oif else #direction = 1 G1 X[#x0] A0 F[#horizontal_feedrate] Oif endif Oif if [ #z LE [#z0 - #depth] ] Oloop break Oif endif Oloop endwhile Owithdraw call [#safez] G0 X[#x1] G0 A0 (go to 0 degree) Othread_on_fourth_axis endsub M2 |
#3
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
Nice - to bad you can't use a hob ? I think that what thread cutters
are or Cob... They have cutters a foot long and 6" in diameter - coated and all - here in Lufkin - the foundry at Lufkin Industries has to do it all. Massive gears and massive bolts and nuts. The traditional donkey that pumps out oil is twice as long as those made by Lufkin. Their custom way saves space and when in buildings (hiding the pump) it becomes important. Martin On 3/21/2013 7:45 PM, Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i |
#4
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On 2013-03-22, Martin Eastburn wrote:
Nice - to bad you can't use a hob ? I think that what thread cutters are or Cob... They have cutters a foot long and 6" in diameter - coated and all - here in Lufkin - the foundry at Lufkin Industries has to do it all. Massive gears and massive bolts and nuts. Yes, to do it properly, I would need to orient the rotary table at angle to axis X. Too difficult for me to do it. I will mess with making threads to see how geometry affects fit and how I can compensate by fudging the diameter. i The traditional donkey that pumps out oil is twice as long as those made by Lufkin. Their custom way saves space and when in buildings (hiding the pump) it becomes important. Martin On 3/21/2013 7:45 PM, Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i |
#5
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNCmill with LinuxCNC
Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? |
#6
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNCmill with LinuxCNC
On Mar 21, 6:49*pm, "Pete C." wrote:
Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? iggy offered the person selling the $1 thread mill ten cents. |
#7
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNCmill with LinuxCNC
On 2013-03-22, Pete C. wrote:
Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? I have not! But I should start looking. i |
#8
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNCmill with LinuxCNC
On Thu, 21 Mar 2013 21:31:19 -0500, Ignoramus3931
wrote: On 2013-03-22, Pete C. wrote: Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? I have not! But I should start looking. i twice now, the auctioneer has called them taps. Makes for a really good deal, I got one lot of 30 "taps" for $100. Even overheard one guy saying that guy was crazy bidding $100 on taps. Karl |
#9
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNCmill with LinuxCNC
Karl Townsend wrote: On Thu, 21 Mar 2013 21:31:19 -0500, Ignoramus3931 wrote: On 2013-03-22, Pete C. wrote: Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? I have not! But I should start looking. i twice now, the auctioneer has called them taps. Makes for a really good deal, I got one lot of 30 "taps" for $100. Even overheard one guy saying that guy was crazy bidding $100 on taps. Karl So you have some extras to sell? |
#10
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNCmill with LinuxCNC
So you have some extras to sell? Unlike iggy, I'm not good at selling things. I do plan to have the best estate auction anybody has ever seen. I think, he who dies with the most toys, wins. karl |
#11
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNCmill with LinuxCNC
On 2013-03-22, Karl Townsend wrote:
On Thu, 21 Mar 2013 21:31:19 -0500, Ignoramus3931 wrote: On 2013-03-22, Pete C. wrote: Ignoramus3931 wrote: My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i Nice, but haven't you found a thread mill for $1 yet? I have not! But I should start looking. i twice now, the auctioneer has called them taps. Makes for a really good deal, I got one lot of 30 "taps" for $100. Even overheard one guy saying that guy was crazy bidding $100 on taps. Karl Yep, definitely fun to listen to comments like thhis! |
#12
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
"Ignoramus3931" wrote in message ... My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. For a 1MM pitch, a hand ground, single point hss threading tool probably would have worked just as well and would also have produced the correct root geometry. |
#13
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 12:52*pm, "PrecisionmachinisT"
wrote: "Ignoramus3931" wrote in ... My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. For a 1MM pitch, a hand ground, single point hss threading tool probably would have worked just as well and would also have produced the correct root geometry. That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. |
#14
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 8:28*pm, jon_banquer wrote:
That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. Maybe not the same as your skills, but a skill never the less. Dan |
#15
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 5:39*pm, " wrote:
On Mar 22, 8:28*pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. *Maybe not the same as your skills, but a skill never the less. Dan Buying stuff for nothing is not a creative process. It's just business. |
#16
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 8:50*pm, jon_banquer wrote:
On Mar 22, 5:39*pm, " wrote: On Mar 22, 8:28*pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. *Maybe not the same as your skills, but a skill never the less. Dan Buying stuff for nothing is not a creative process. It's just business. Any five-finger discounts in that, as I assume? |
#17
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
|
#18
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 6:15*pm, Ignoramus6048
wrote: On 2013-03-23, wrote: On Mar 22, 8:28?pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. *Maybe not the same as your skills, but a skill never the less. Thanks. Converting a Bridgeport milling machine to Linux is also a skill. And yapping on forums about "having access to a friend's shop" is not a skill. As for single point threading, my current problem is that the spindle has to be on brake. However, spindle brake right now is tied to estop. It only activates when the mill is e-stopped, and deactivates when the mill is out of estop. Fixing that requires me to spend a considerable time writing emc2 logic statements (to interlock brake and estop and spindle running safely). I do not have time for this right now. i iggy has very few metalworking or welding skills even after many years of posting here. He's a butcher/hack with no clues. Gaining skills means paying your dues. iggy refuses to pay his dues and he has no respect for others such as Precision Machinist. iggy has kill filled Precision Machinist who, unlike Mark Wieber, refuses to coddle and spoon feed iggy. The sad fact is that iggy can't handle anyone who tells him the truth about his ****ed up approach to metalworking and welding. He's on a series ego trip that for years has prevented him from properly learning and acquiring the needed metalworking and welding skills and it shows in almost every post iggy makes. |
#19
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On Mar 22, 6:15*pm, Ignoramus6048
wrote: On 2013-03-23, wrote: On Mar 22, 8:28?pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. *Maybe not the same as your skills, but a skill never the less. Thanks. Converting a Bridgeport milling machine to Linux is also a skill. And yapping on forums about "having access to a friend's shop" is not a skill. As for single point threading, my current problem is that the spindle has to be on brake. However, spindle brake right now is tied to estop. It only activates when the mill is e-stopped, and deactivates when the mill is out of estop. Fixing that requires me to spend a considerable time writing emc2 logic statements (to interlock brake and estop and spindle running safely). I do not have time for this right now. i "And yapping on forums about "having access to a friend's shop" is not a skill" Jealousy isn't a skill either, douchebag. Neither is your bitching about the kind or prices I get for some of the tools I sell in the lame e-mails you have sent me in the past. |
#20
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
"Ignoramus6048" wrote in message ... On 2013-03-23, wrote: On Mar 22, 8:28?pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. Maybe not the same as your skills, but a skill never the less. Thanks. Converting a Bridgeport milling machine to Linux is also a skill. And yapping on forums about "having access to a friend's shop" is not a skill. As for single point threading, my current problem is that the spindle has to be on brake. No, it doesn't. However, spindle brake right now is tied to estop. It only activates when the mill is e-stopped, and deactivates when the mill is out of estop. Fixing that requires me to spend a considerable time writing emc2 logic statements (to interlock brake and estop and spindle running safely). I do not have time for this right now. i |
#21
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
On Fri, 22 Mar 2013 17:39:49 -0700 (PDT), "
wrote: On Mar 22, 8:28Â*pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. Maybe not the same as your skills, but a skill never the less. Dan Indeed it is. Very much of a skill..and it can be a high dollar one at that. Gunner |
#22
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
"Gunner Asch" wrote in message
... On Fri, 22 Mar 2013 17:39:49 -0700 (PDT), " wrote: On Mar 22, 8:28 pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. Maybe not the same as your skills, but a skill never the less. Dan Indeed it is. Very much of a skill..and it can be a high dollar one at that. Gunner I have the knack for buying at 5% of value but unfortunately never acquired the salesman skills to sell for much more than that. jsw |
#23
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
Gunner Asch on Fri, 22 Mar 2013 20:44:15 -0700
typed in rec.crafts.metalworking the following: On Fri, 22 Mar 2013 17:39:49 -0700 (PDT), " wrote: On Mar 22, 8:28*pm, jon_banquer wrote: That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. Buying stuff for nothing is a skill. Maybe not the same as your skills, but a skill never the less. Dan Indeed it is. Very much of a skill..and it can be a high dollar one at that. Yep, heard of a guy who was buying stuff for a dollar and selling it for two dollars, sometimes three. He said it was amazing how that one to two percent markup really added up. I decided not to enlighten him... -- pyotr filipivich "With Age comes Wisdom. Although more often, Age travels alone." |
#24
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On 3/22/2013 20:28, jon_banquer wrote:
On Mar 22, 12:52 pm, "PrecisionmachinisT" wrote: "Ignoramus3931" wrote in ... My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. For a 1MM pitch, a hand ground, single point hss threading tool probably would have worked just as well and would also have produced the correct root geometry. That would require building a skill. That's not iggy's bag. iggy is almost totally focused on buying stuff for nothing rather than building skills. I would say converting a machine to a different control, and writing complex routines for doing unusual things with it constitute a real skill. Don't forget his math abilities, second to nobody in this group. He seems to find a LOT of spare time to enjoy doing things other than buying and selling. Check out his website, totally voluntary done by him. People really only need to learn skills to complete the task at hand. Read some of his posts about what he HAS done, and see how many you can do. Sure, others may have different skillsets, but those who can and do, and also post proof, are way above and beyond those who only brag. I would much prefer to see all that people have done, than just read in this newsgroup about stuff people have done. "It ain't braggin' if you can do it." -- Yogi Berra I wish I had enough spare time to do more, but gotta balance work, family, rest, etc. What's left over my spare time. G -- Steve Walker (remove brain when replying) |
#25
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport Interact CNC mill with LinuxCNC
"Ignoramus3931" wrote in message
... My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i That's great! I guess it would also work to make rifling guides, like 1 revolution in 9 inches or so? RogerN |
#26
Posted to rec.crafts.metalworking
|
|||
|
|||
VIDEO of cutting a thread on 4th axis of my Bridgeport InteractCNC mill with LinuxCNC
On 2013-03-24, RogerN wrote:
"Ignoramus3931" wrote in message ... My guy asked me to cut a 1mm pitch thread on a custom shaft. I could not do it on my lathe, so I finally bit the bullet and wrote a subroutine to do threading with my 4th axis rotary table. I use a 60 degree chamfering end mill. Now I can cut any thread, any pitch, right or left handed, and if the thread is very coarse, the subroutine does it in several passes. http://www.youtube.com/watch?v=JMENnIJrl9Y I am afraid that it does not create a 100% correct thread geometry, but I hope that I can do enough things with it to be useful with some adjustments to diameter. i That's great! I guess it would also work to make rifling guides, like 1 revolution in 9 inches or so? Sure, it could not care less if the step is 1 revolition per 9 inch or 0.09 inch. It does the same thing. By default, it calculates depth based on 60 degree thread profile, but you can specify your desired depth. i |
Reply |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Forum | |||
Bridgeport Interact 1 Heidehain Controls | Metalworking | |||
Bridgeport Series II Interact 2 back gear ratio | Metalworking | |||
Bridgeport Interact 2 tapping capacity | Metalworking | |||
Cost of the Bridgeport Interact 2 mill dropped down to $5 (sic) | Metalworking | |||
Looking for help with a Bridgeport Interact I MK2 | Metalworking |