| Page 1 of 2 | 1 | 2 |
|
|
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
I bought a couple of 3/4" thick aluminum fixture plates.
http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 17:34:44 -0500, Karl Townsend
wrote: On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl sorry you had two more queries. I used a solid holder, your floating holder would be nice. Spot drill if you need to hold +/- .002 location, stub drill maybe +/- ..005, regular drill maybe +/- .010 or worse. So how accurate determines answer. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Gene wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. That depends on the drill and the material. HSS drill? Maybe 2500 RPM and maybe .005 per rev feed. That is a bit conservative, but I'd prefer to finish without a lot of tool changing. Pecking once will probably be sufficient. Not bad. 80 rev per secons and 0.005 per rev means 0.4 inch per second. Would the stringy chips want to wrap around the drill bit? Be wary, though, of scoring "good deals" in material. If this isn't cast tooling plate, but some soft sticky stuff more akin to 1100, you'll have your hands full. Use a cutting fluid. I will use flood coolant in large amounts. his plate alteady has a few smaller holes drilled and tapped. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. Absolutely, if nothing else, done properly, they provide the chamfer for the finished thread. Great. I am thinking, use a spotting drill, and drill a full diameter hole that is perhaps 1/8" deep. That would provide good centering. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html Sure. Go for it. However, again, if you have inherited some suspicious material, say one of the 6xxx materials.... you'll dull taps VERY quickly and a tap burner or scrap will be in your immediate future. Well, it is already tapped, so it is tappable. ix |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 17:34:44 -0500, Karl Townsend wrote: On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl sorry you had two more queries. I used a solid holder, your floating holder would be nice. Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, regular drill maybe +/- .010 or worse. So how accurate determines answer. Karl I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill. i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl Pretty cool. You feed 5.1 is how many inches per second? Someone suggested 0.4 IPS, which makes some sense to me. i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898
wrote: On 2010-09-26, Karl Townsend wrote: On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl Pretty cool. You feed 5.1 is how many inches per second? Someone suggested 0.4 IPS, which makes some sense to me. i That's 5.1 IPM. I just looked at the math, probably could have doubled the feed. Only four holes, chips were feeding, don't **** with it. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Karl Townsend wrote:
On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898 wrote: On 2010-09-26, Karl Townsend wrote: On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 wrote: I bought a couple of 3/4" thick aluminum fixture plates. http://igor.chudov.com/tmp/Fixture-Plate.jpg It was a local sale. I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Karl Pretty cool. You feed 5.1 is how many inches per second? Someone suggested 0.4 IPS, which makes some sense to me. i That's 5.1 IPM. I just looked at the math, probably could have doubled the feed. Only four holes, chips were feeding, don't **** with it. Just trying to do the math. 5 IPM, means one 1" hole drilled in 12 seconds, so it amounts to about 20 seconds per hole with rapids and everything. 200 holes, means 4,000 seconds, a little over an hour. Probably can run unsupervised. Not too bad. How bad were the chips? i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
Great. I am thinking, use a spotting drill, and drill a full diameter hole that is perhaps 1/8" deep. That would provide good centering. If you use 60 degree center drill and go to a depth of half the hole diameter of the 3/8 thread diameter the finished hole will have a nice chamfer on it with no need for any deburring. John |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
Ignoramus24898 writes:
I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success. If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87). Now you know why these cost $$$$: http://www.edmundoptics.com/onlineca...productID=2929 |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote: Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, regular drill maybe +/- .010 or worse. So how accurate determines answer. I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill. Is a "spot drill" the same thing as a "center drill"? (it kind of sounds like it, from Karl's info here.) Thanks, Rich |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote: On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898 Some questions. 1. What is the best way to drill aluminum with 5/16" drill bit, making through holes. What RPM and feedrate and how often to peck. 2. Do I need to center drill those holes first? It is not really a big deal, just some more G codes. 3. For tapping, can I safely use a ER colleted floating tap holder that has a little bit of vertical internal travel. Like this one: http://www.maritool.com/p67/ER25-Flo...duct_info.html By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow. Pretty cool. You feed 5.1 is how many inches per second? Someone suggested 0.4 IPS, which makes some sense to me. This makes me wonder: Is there a machine where a machinist could make one part "by hand", i.e., in the normal way you'd use a regular mill or whatever, but where the machine could record the machinist's actions, and then "play them back" for the next part? Or is it only possible to drive an NC by writing a string of textual commands? Thanks, Rich |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sep 26, 10:23*pm, Ignoramus24898
Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, *regular drill maybe +/- .010 or worse. So how accurate determines answer. Karl I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill. i If I were doing this on a manual mill, I would spot drill with a drill whose diameter is about the size of the web of the drill used for the hole. Dan |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sun, 26 Sep 2010 23:32:26 -0700, Rich Grise
wrote: On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote: On 2010-09-26, Karl Townsend wrote: Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, regular drill maybe +/- .010 or worse. So how accurate determines answer. I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill. Is a "spot drill" the same thing as a "center drill"? (it kind of sounds like it, from Karl's info here.) Thanks, Ric No, they are different. A spot drill looks like a drill bit with a special grind point. |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
This makes me wonder: Is there a machine where a machinist could make one part "by hand", i.e., in the normal way you'd use a regular mill or whatever, but where the machine could record the machinist's actions, and then "play them back" for the next part? Or is it only possible to drive an NC by writing a string of textual commands? My control has a "teach" mode to record points but you still eidt to make a program. I never used one but the bridegeport protrack was supposed to do this. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Karl Townsend wrote:
How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Karl Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? Thanks i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Richard J Kinch wrote:
Ignoramus24898 writes: I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success. If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87). Now you know why these cost $$$$: http://www.edmundoptics.com/onlineca...productID=2929 Richard, I was hoping that I would tap on my CNC mill, so whatever process I do, would be repeatable and not as random as manual tapping. i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sep 27, 8:26*am, Ignoramus21149 ignoramus21...@NOSPAM.
21149.invalid wrote: On 2010-09-27, Richard J Kinch wrote: Ignoramus24898 writes: I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? *If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. *For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success. If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87). Now you know why these cost $$$$: http://www.edmundoptics.com/onlineca...t.cfm?productI... Richard, I was hoping that I would tap on my CNC mill, so whatever process I do, would be repeatable and not as random as manual tapping. i- Hide quoted text - - Show quoted text - For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. _kevin |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
"Ignoramus21149" wrote in message ... On 2010-09-27, Karl Townsend wrote: How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Karl Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? Thanks i If they are through holes, I would go with a gun tap - they push the chips ahead of the tap. I have a Procunier tapping head you could borrow for a week or so if that would help. I've tapped a bunch of 0-80 and 4-40 holes with nary a broken tap so 5/16" shouldn't be a problem for that style of head. Mike |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, karchiba wrote:
For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. That's a good idea. Would you say, with a proper tin coated tap like this, and using a letter S drill, the 3/8" holes can be tapped consistently on my CNC mill? i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Mike Henry wrote:
"Ignoramus21149" wrote in message ... On 2010-09-27, Karl Townsend wrote: How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Karl Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? Thanks i If they are through holes, I would go with a gun tap - they push the chips ahead of the tap. I have a Procunier tapping head you could borrow for a week or so if that would help. I've tapped a bunch of 0-80 and 4-40 holes with nary a broken tap so 5/16" shouldn't be a problem for that style of head. Mike, did you use that head on a CNC mill? |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? I don't agree with Richard's analysis. His method assumes the probabilty of a broken tap is the same on every hole. In fact, once you've set up proper conditions and selected a top quality tap the probablity of breaking goes with wear. Taps used in machines last FAR longer than hand taps. I use OSG brand taps. Gun flute on thru hole, spiral flute on blind hole. I forget, you aren't set up for rigid tapping?? Both your tension/compression tap holder and the procunier can be set up in your CNC. But, its tricky. You've got to match feeds and speeds to where the tap wants to be. Karl |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Karl Townsend wrote:
Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? I don't agree with Richard's analysis. His method assumes the probabilty of a broken tap is the same on every hole. In fact, once you've set up proper conditions and selected a top quality tap the probablity of breaking goes with wear. Taps used in machines last FAR longer than hand taps. OK, good to hear. I use OSG brand taps. Gun flute on thru hole, spiral flute on blind hole. I forget, you aren't set up for rigid tapping?? Both your tension/compression tap holder and the procunier can be set up in your CNC. But, its tricky. You've got to match feeds and speeds to where the tap wants to be. I understand, yes. If I run the spindle at, say, 200-300 RPM, then it would take me about 0.2 seconds to stop the spindle, so about one revolution. The floating tap holder should be able to take care of that. You think ER16 collets would hold a tap well enough? i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, Karl Townsend wrote: Karl, thanks. I will try on some aluminum junk that I have, first. Tapping, as Richard noted, may be a challenge. What tap would you recommend for this (tapping aluminum)? I don't agree with Richard's analysis. His method assumes the probabilty of a broken tap is the same on every hole. In fact, once you've set up proper conditions and selected a top quality tap the probablity of breaking goes with wear. Taps used in machines last FAR longer than hand taps. OK, good to hear. I use OSG brand taps. Gun flute on thru hole, spiral flute on blind hole. I forget, you aren't set up for rigid tapping?? Both your tension/compression tap holder and the procunier can be set up in your CNC. But, its tricky. You've got to match feeds and speeds to where the tap wants to be. I understand, yes. If I run the spindle at, say, 200-300 RPM, then it would take me about 0.2 seconds to stop the spindle, so about one revolution. The floating tap holder should be able to take care of that. You think ER16 collets would hold a tap well enough? I wrote a G-code subroutine to do it. To run safely, it MUST have a floating tap holder that can take up the slack of the tap that moves off position, while the spindle is reversed. (Tap a hole with a floating holder) Otap_with_floating_holder sub #depth = #1 (Hole Depth) #tpi = #2 (Threads per Inch) #rpm = #3 (RPM of the spindle, EXACTLY MEASURED) #safez = #4 (Safe Height) #frate = [#rpm / #tpi] M3 (Forward) G1 Z#depth F#frate M4 (Reverse) G1 Z#safez F#frate M3 (Forward again) Otap_with_floating_holder endsub M2 |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Sep 26, 11:11*pm, Richard J Kinch wrote:
Ignoramus24898 writes: I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? *If you're not an utterly reliable tapper, you'll never be able to complete this job. So, make threaded inserts of steel, for oversized holes (stepped would be good) with a bit of loctite. The accuracy of a screw position isn't critical, I trust. Of course, to churn out inserts might require a CNC lathe... or a turret lathe. |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Mon, 27 Sep 2010 07:12:36 -0500, Karl Townsend wrote:
On Sun, 26 Sep 2010 23:32:26 -0700, Rich Grise On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote: On 2010-09-26, Karl Townsend wrote: Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, regular drill maybe +/- .010 or worse. So how accurate determines answer. I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill. Is a "spot drill" the same thing as a "center drill"? (it kind of sounds like it, from Karl's info here.) No, they are different. A spot drill looks like a drill bit with a special grind point. Ah. Thanks. I sit in an office and fly a desk, while right outside my door are a couple of machinists and weldors - on one side of the shop, we take big pieces of metal and turn them into little pieces of metal, and on the other side, we take small pieces of metal and turn them into big pieces of metal. :-) On break, the only people I have to talk to, other than the boss and his secretary, are the machinists - When I'm chatting someone up, I like to be able to speak the same language as they. :-) I do know what "spot-facing" is, however. ;-) Thanks! Rich |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
|
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote:
How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Once, after hours, I found some really spiffy pieces of aluminum out in back next to the bandsaw. I wanted to make a trinket, and the resident machinist taught me how to use a mill - I was astonished how much metal he could hog off that aluminum block; Previously, as a hobbyist, I had used about a quarter the feed rate this guy was getting away with. I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of 304SS. I din't even know you _could_ drill 304SS with an ordinary twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore down on that handle thingie that extends the quill, and the stainless just gave way. I heard that sound that you hear when one mongo chip is being produced, and it felt almost like the drill was pulling itself into the work - I was through 3/16 of metal in a matter of seconds, almost effortlessly! So, I guess I'd have to admit, when I'm playing with metal, I should be more aggressive with my cuts. :-) I once saw a guy deburr a steel part with an ordinary pocket knife. Does that dull the knife? How can steel cut steel? Howcome the part doesn't cut the bit? Thanks, Rich |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 09/27/2010 12:40 PM, Ignoramus21149 wrote:
I wrote a G-code subroutine to do it. To run safely, it MUST have a floating tap holder that can take up the slack of the tap that moves off position, while the spindle is reversed. (Tap a hole with a floating holder) Otap_with_floating_holder sub #depth = #1 (Hole Depth) #tpi = #2 (Threads per Inch) #rpm = #3 (RPM of the spindle, EXACTLY MEASURED) #safez = #4 (Safe Height) #frate = [#rpm / #tpi] M3 (Forward) G1 Z#depth F#frate M4 (Reverse) G1 Z#safez F#frate M3 (Forward again) Otap_with_floating_holder endsub M2 Well, this all SOUNDS good, but in fact, there is NO connection, at all, between the spindle and the Z feed. You'd have to do the first test holes carefully to make sure you get the desired depth of tapping. The spindle is running at whatever speed it is, and the Z infeed goes at the programmed rate. But, at the end, it is only the Z depth that determines when to reverse. NOT, the number of turns the tap has fed into the work. Still, this is likely to work, assuming the springs on the tap holder are strong enough to start the tap into the work promptly. And, you won't believe what a MESS this will make, if you ever mess up and have the spindle running at the wrong speed for the calculated feedrate. been there, done that! Jon |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On Mon, 27 Sep 2010 07:22:47 -0500, Karl Townsend wrote:
This makes me wonder: Is there a machine where a machinist could make one part "by hand", i.e., in the normal way you'd use a regular mill or whatever, but where the machine could record the machinist's actions, and then "play them back" for the next part? Or is it only possible to drive an NC by writing a string of textual commands? My control has a "teach" mode to record points but you still eidt to make a program. I never used one but the bridegeport protrack was supposed to do this. Thanks; I was just curious, but it sounds like a fascinating opportunity for a geek like me (microprocessor programmer) who dabbles in mechanical stuff... Thanks! Rich |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 09/27/2010 10:13 AM, Ignoramus21149 wrote:
On 2010-09-27, wrote: For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. That's a good idea. Would you say, with a proper tin coated tap like this, and using a letter S drill, the 3/8" holes can be tapped consistently on my CNC mill? i You use an entirely different drill size (much larger) for a thread forming tap. The workpiece is pushed out of the peaks to form the valleys. The tap manufacturer should be able to recommend the correct drill size. Jon |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Jon Elson wrote:
On 09/27/2010 12:40 PM, Ignoramus21149 wrote: I wrote a G-code subroutine to do it. To run safely, it MUST have a floating tap holder that can take up the slack of the tap that moves off position, while the spindle is reversed. (Tap a hole with a floating holder) Otap_with_floating_holder sub #depth = #1 (Hole Depth) #tpi = #2 (Threads per Inch) #rpm = #3 (RPM of the spindle, EXACTLY MEASURED) #safez = #4 (Safe Height) #frate = [#rpm / #tpi] M3 (Forward) G1 Z#depth F#frate M4 (Reverse) G1 Z#safez F#frate M3 (Forward again) Otap_with_floating_holder endsub M2 Well, this all SOUNDS good, but in fact, there is NO connection, at all, between the spindle and the Z feed. The only connection is that I measure the speed of the spindle with a handheld tachometer, and then calculate the feed. You'd have to do the first test holes carefully to make sure you get the desired depth of tapping. The spindle is running at whatever speed it is, and the Z infeed goes at the programmed rate. But, at the end, it is only the Z depth that determines when to reverse. NOT, the number of turns the tap has fed into the work. Absolutely. Still, this is likely to work, assuming the springs on the tap holder are strong enough to start the tap into the work promptly. And, you won't believe what a MESS this will make, if you ever mess up and have the spindle running at the wrong speed for the calculated feedrate. been there, done that! What will happen, it will tear the tap out of the collet? Anyway, obviously rigid tapping, optionally with the floating holder, is the way to go. i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Jon Elson wrote:
On 09/27/2010 10:13 AM, Ignoramus21149 wrote: On 2010-09-27, wrote: For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. That's a good idea. Would you say, with a proper tin coated tap like this, and using a letter S drill, the 3/8" holes can be tapped consistently on my CNC mill? i You use an entirely different drill size (much larger) for a thread forming tap. The workpiece is pushed out of the peaks to form the valleys. The tap manufacturer should be able to recommend the correct drill size. Yep. I will buy a form tap today at mcmaster, they say use letter S drill. i |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
Rich Grise wrote:
On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote: How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Once, after hours, I found some really spiffy pieces of aluminum out in back next to the bandsaw. I wanted to make a trinket, and the resident machinist taught me how to use a mill - I was astonished how much metal he could hog off that aluminum block; Previously, as a hobbyist, I had used about a quarter the feed rate this guy was getting away with. I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of 304SS. I din't even know you _could_ drill 304SS with an ordinary twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore down on that handle thingie that extends the quill, and the stainless just gave way. I heard that sound that you hear when one mongo chip is being produced, and it felt almost like the drill was pulling itself into the work - I was through 3/16 of metal in a matter of seconds, almost effortlessly! So, I guess I'd have to admit, when I'm playing with metal, I should be more aggressive with my cuts. :-) And never ease off the pressure until you are at depth or through the other side. Many steels will work-harden in an instant if you let the drill spin and not cut. |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 9/27/2010 3:08 PM, Rich Grise wrote:
On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote: How bad were the chips? I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best. You should feed maybe twice as fast as my small run. Once, after hours, I found some really spiffy pieces of aluminum out in back next to the bandsaw. I wanted to make a trinket, and the resident machinist taught me how to use a mill - I was astonished how much metal he could hog off that aluminum block; Previously, as a hobbyist, I had used about a quarter the feed rate this guy was getting away with. I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of 304SS. I din't even know you _could_ drill 304SS with an ordinary twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore down on that handle thingie that extends the quill, and the stainless just gave way. I heard that sound that you hear when one mongo chip is being produced, and it felt almost like the drill was pulling itself into the work - I was through 3/16 of metal in a matter of seconds, almost effortlessly! So, I guess I'd have to admit, when I'm playing with metal, I should be more aggressive with my cuts. :-) I once saw a guy deburr a steel part with an ordinary pocket knife. Does that dull the knife? How can steel cut steel? Howcome the part doesn't cut the bit? There's hard steel, and there's soft steel. The hard steel cuts the soft steel. -- I can see November from my front porch |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Richard J Kinch wrote:
Ignoramus24898 writes: I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success. If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87). I think, with the proper coolant/lubricant, good gun (spiral point) taps, and the consistency of the CNC, he might be able to do this with no problems -- with a high quality tap and a good hard aluminum alloy. I would either use a TapMagic for aluminum, or just use WD-40 in aluminum. Even better for the task would be a TapMatic tap head (which would eliminate the problem of feeding in reverse as you back the tap out). The thing with at least some models of TapMatic heads is a friction clutch, which you set up with a brand new tap so is just barely does not slip when cutting with the proper lubricant. Then, once the tap starts getting dull, it will slip and you can change out the tap *before* it breaks. I've used this setup in a drill press with 1/4-20 HSS gun taps with 1/4" steel (making an apron for an old DiAcro sheet metal shear). Now you know why these cost $$$$: http://www.edmundoptics.com/onlineca...productID=2929 Hmm ... the code which that website has which wants to know where I live is a pain. I can't find the right things to turn on to get it to accept my data (cookies and JavaScript on, and it still refuses to admit that I've given it a value and keeps asking. It probably wants flash, which I refuse to turn on. So -- I had to start over and click the [dismiss] button to get anywhere since it would not let me back out to the original starting point. Enjoy, DoN. -- Remove oil spill source from e-mail Email: | Voice (all times): (703) 938-4564 (too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html --- Black Holes are where God is dividing by zero --- |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, karchiba wrote:
On Sep 27, 8:26*am, Ignoramus21149 ignoramus21...@NOSPAM. 21149.invalid wrote: On 2010-09-27, Richard J Kinch wrote: Ignoramus24898 writes: I would like to drill and tap them with 5/16" drill and 3/8" tap, say spaced at 1" interval. That makes for about 200 holes to be drilled and tapped on my CNC mill. How frequently do you break taps? *If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. *For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success. If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87). [ ... ] Richard, I was hoping that I would tap on my CNC mill, so whatever process I do, would be repeatable and not as random as manual tapping. [ ... ] For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. That is a good idea. However -- be sure to look up the right drill size for a thread forming tap. It *has* to be larger than the normal thread cutting tap's tap drill. You say 3/8" holes, but don't say which thread pitch, so I can't look up the drill size. It can be found in _Machinery's Handbook_. The nearest to perfect size for a 1/4-20 tap happens to be a metric size -- 5.7mm -- another argument for having drills of all kinds. The proper size for 10-32 thread forming taps is a #17 -- from your recently acquired number sized drill set. Good Luck, DoN. -- Remove oil spill source from e-mail Email: | Voice (all times): (703) 938-4564 (too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html --- Black Holes are where God is dividing by zero --- |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, karchiba wrote: For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips. That's a good idea. Would you say, with a proper tin coated tap like this, and using a letter S drill, the 3/8" holes can be tapped consistently on my CNC mill? I see that you've found the "Cold Form Tapping" chart in _Machinery's Handbook_ -- and that you are going for 3/8-16 threads, and 65% full thread. The final question is -- what is the proper lubricant for this in aluminum? (And no -- *I* don't know the answer -- I hope someone else here does.) Enjoy, DoN. -- Remove oil spill source from e-mail Email: | Voice (all times): (703) 938-4564 (too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html --- Black Holes are where God is dividing by zero --- |
Drilling and tapping 200+ 3/8" holes in 3/4" aluminum
On 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, Karl Townsend wrote: [ ... ] I don't agree with Richard's analysis. His method assumes the probabilty of a broken tap is the same on every hole. In fact, once you've set up proper conditions and selected a top quality tap the probablity of breaking goes with wear. Taps used in machines last FAR longer than hand taps. OK, good to hear. I use OSG brand taps. Gun flute on thru hole, spiral flute on blind hole. I forget, you aren't set up for rigid tapping?? Both your tension/compression tap holder and the procunier can be set up in your CNC. But, its tricky. You've got to match feeds and speeds to where the tap wants to be. I understand, yes. If I run the spindle at, say, 200-300 RPM, then it would take me about 0.2 seconds to stop the spindle, so about one revolution. The floating tap holder should be able to take care of that. But you *really* should keep feeding according to the revolution of the spindle on the index until it stops -- so your machine knows where the tap is when it starts in reverse. You think ER16 collets would hold a tap well enough? The typical tapping head has a special chuck. It uses two ways to hold the tap. A Jacobs Rubberflex type collet to assure concentricity and a pair of plates with a combination left and right hand threaded leadscrew connecting them to clamp down on the flats on the end of the tap shank. Some floating tap holders have similar chucks. The main thing to consider is -- if it *does* slip and you are doing rigid tapping, it will no longer be at the right depth for the number of turns which the tap has taken. I would look for something with the Jacobs tap chuck for this, myself. And the Procunier or TapMatic tapping heads have them, along with other features which make machine tapping easier -- including automatic reversing when you start to back out of the hole -- while the spindle is still turning clockwise. :-) When doing tapping with a releasing tap holder in the bed turret of my manual lathe, I've made tap holders which are simply the right diameter for the shank of the tap, and a pair of setscrews opposite each other to clamp on two opposing flats. Good luck, DoN. -- Remove oil spill source from e-mail Email: | Voice (all times): (703) 938-4564 (too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html --- Black Holes are where God is dividing by zero --- |
| All times are GMT +1. The time now is 08:35 PM. |
|
Powered by vBulletin® Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.
Copyright ©2004 - 2014 DIYbanter